| Page 1 of 2 | 1 | 2 |
|
|
Better luck machining aluminum
I have decided to dial way down this time. Again, I am making a mold
cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i |
Better luck machining aluminum
Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping. I can't see your G-code, but forget the coolant and try something like 1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end mill this is only like 0.005" chip load, very conservative. Watch how it cuts at that feed rate and try the feed rate override to bump the feed up if it looks happy. You have a 2-3 HP machine, you should not be taking cuts that are a fraction of what my 1 HP machine happily takes. |
Better luck machining aluminum
"Pete C." wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping. I can't see your G-code, but forget the coolant and try something like 1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end mill this is only like 0.005" chip load, very conservative. Watch how it cuts at that feed rate and try the feed rate override to bump the feed up if it looks happy. You have a 2-3 HP machine, you should not be taking cuts that are a fraction of what my 1 HP machine happily takes. Take a look at: http://wpnet.us/nn_clone/index.htm Pretty much all of that aluminum was machined dry on my wee little 1J Bridgeport (except of course for the parts turned dry on my lathe). The only place coolant was used was on the engraving with a tiny carbide engraving bit. |
Better luck machining aluminum
"Pete C." fired this volley in news:4c522b8e$0$10427
: but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. LLoyd |
Better luck machining aluminum
"Pete C." wrote in message ster.com... Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping. agree with the above - with the last piece of aluminum I machined on my Abene mill, I needed a 1/2 inch by 3/4 inch deep rabbet around the edges of a slab - I put in a 1 inch end mill at whatever my table of RPM said for aluminum and milled it in a single pass, I think I had the feed set to 4 inches per minute, but it's been a while - worked perfectly. of course this is a manual mill, not CNC, but that shouldn't matter |
Better luck machining aluminum
On Jul 29, 6:42*pm, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote: "Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. LLoyd I also agree wit no coolant necessary. I do lots of milling on 1/4 tooling plates of 6061. I began with mist coolant, but the mister leaked, so I stored it in an old plastic waste basket. One day the janitor spotted it and threw it out. It was in a waste basket, right? Since then I mill dry with two-flute end mills. Almost all my work is completely through the plate, so chips are not usually a problem. In your case, they will be. Can you rig up a shop vacuum to suck out the chips? That and a 1" chip brush will get the job done. Paul |
Better luck machining aluminum
"Ignoramus5687" wrote in message ... I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i I had pretty good luck machining aluminum with an end mill made for aluminum and a mist coolant setup. I think the mist coolant system mainly helped by blowing chips away from the cutter. My end mill was a 3 flute for aluminum that I bought from McMaster Carr IIRC. The 3 flutes gave more strength than 2 flute and more chip clearance than a 4 flute, or at least the ad said something to that effect. It's time to put Quincy to work! RogerN |
Better luck machining aluminum
On 2010-07-30, Ignoramus5687 wrote:
Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. Actually I have decided to make a pump from the mill to work. It is inside the mill's base. It is not that hard to get to, through the side door. I will make the coolant pump controlled by EMC instead of just the panel switch. That way I will be able to turn on coolant with M8 command. The weird thing is that there is liquid in the sump now, but it seems to be straight oil. Once I get it to work, hopefully tonight, I will pump it all out and look. It may be all the lubricating oil from the ways that accumulated. i |
Better luck machining aluminum
On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. OK, that's good. I guess I was just spinning the cutter too fast. i |
Better luck machining aluminum
|
Better luck machining aluminum
Ignoramus5687 wrote:
I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. That oil in your sump is probably an oil-based coolant. Might be even messier than water-based, but it probably works fine, too. Jon |
Better luck machining aluminum
On 2010-07-30, RogerN wrote:
"Ignoramus5687" wrote in message ... I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i I had pretty good luck machining aluminum with an end mill made for aluminum and a mist coolant setup. I think the mist coolant system mainly helped by blowing chips away from the cutter. My end mill was a 3 flute for aluminum that I bought from McMaster Carr IIRC. The 3 flutes gave more strength than 2 flute and more chip clearance than a 4 flute, or at least the ad said something to that effect. It's time to put Quincy to work! Roger, just how far do the chips fly? i |
Better luck machining aluminum
Ignoramus5687 wrote: On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote: "Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. OK, that's good. I guess I was just spinning the cutter too fast. i No, it's difficult to spin it too fast really, but the feed rate needs to be appropriate for the cutter RPM. Again it comes down to the chip load, i.e. the amount of material removed by each flute of the end mill each time it rotates around, which is a function of the RPM, feed rate and number of flutes. Chances are you were feeding far too slow on that first attempt, which resulted in very thin chips which stayed in the cut area and got mashed together gumming everything up. I lost track of where that post was, but you can certainly calculate what your chip load was for it and I bet it was 0.001" or less which is far too low. |
Better luck machining aluminum
Ignoramus5687 wrote: On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote: "Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. OK, that's good. I guess I was just spinning the cutter too fast. i Additionally, note that there are a lot of folks out there cutting aluminum dry, with a CNC router spinning a bit at 20,000 RPM and moving at quite high feed rates on home built CNC routers. You can find a bunch of these online. |
Better luck machining aluminum
On 2010-07-30, Pete C. wrote:
"Pete C." wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping. I can't see your G-code, but forget the coolant and try something like 1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end mill this is only like 0.005" chip load, very conservative. Watch how it cuts at that feed rate and try the feed rate override to bump the feed up if it looks happy. You have a 2-3 HP machine, you should not be taking cuts that are a fraction of what my 1 HP machine happily takes. Take a look at: http://wpnet.us/nn_clone/index.htm Pretty much all of that aluminum was machined dry on my wee little 1J Bridgeport (except of course for the parts turned dry on my lathe). The only place coolant was used was on the engraving with a tiny carbide engraving bit. Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. i |
Better luck machining aluminum
On 2010-07-30, Jon Elson wrote:
Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. That oil in your sump is probably an oil-based coolant. Might be even messier than water-based, but it probably works fine, too. No, it is just a mess of way oil that accumulated. i |
Better luck machining aluminum
On 2010-07-30, Pete C. wrote:
Ignoramus5687 wrote: On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote: "Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. OK, that's good. I guess I was just spinning the cutter too fast. i Additionally, note that there are a lot of folks out there cutting aluminum dry, with a CNC router spinning a bit at 20,000 RPM and moving at quite high feed rates on home built CNC routers. You can find a bunch of these online. I saw a video of that, very impressive. i |
Better luck machining aluminum
Ignoramus18915 wrote: On 2010-07-30, Pete C. wrote: "Pete C." wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. i Iggy, it *aluminum*, aluminum is routinely machined dry. Coolant isn't your problem, but it's getting you wrapped around the axle and not focused on where your problem actually is. I machine quite a bit of aluminum and pretty much never use any sort of coolant, or even sprays of WD-40. The only time I use fluids on aluminum is when hand tapping. I can't see your G-code, but forget the coolant and try something like 1200 RPM, 0.100" depth of cut and 10 IPM. If you have a two flute end mill this is only like 0.005" chip load, very conservative. Watch how it cuts at that feed rate and try the feed rate override to bump the feed up if it looks happy. You have a 2-3 HP machine, you should not be taking cuts that are a fraction of what my 1 HP machine happily takes. Take a look at: http://wpnet.us/nn_clone/index.htm Pretty much all of that aluminum was machined dry on my wee little 1J Bridgeport (except of course for the parts turned dry on my lathe). The only place coolant was used was on the engraving with a tiny carbide engraving bit. Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. i Practice with HSS end mills, not brittle carbide ones. |
Better luck machining aluminum
On Fri, 30 Jul 2010 06:51:20 -0500, "Pete C."
wrote the following: Ignoramus5687 wrote: On 2010-07-30, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote: "Pete C." fired this volley in news:4c522b8e$0$10427 : but forget the coolant Well, Iggy, I wouldn't _forget_ the coolant, but I tend to agree with Pete on the last issue. I do a great deal of work in 6061 with no coolant and no problems moving significant amounts of metal -- even with my old BP "M" head, which is fractional HP. OK, that's good. I guess I was just spinning the cutter too fast. i No, it's difficult to spin it too fast really, but the feed rate needs to be appropriate for the cutter RPM. Again it comes down to the chip load, i.e. the amount of material removed by each flute of the end mill each time it rotates around, which is a function of the RPM, feed rate and number of flutes. Chances are you were feeding far too slow on that first attempt, which resulted in very thin chips which stayed in the cut area and got mashed together gumming everything up. I lost track of where that post was, but you can certainly calculate what your chip load was for it and I bet it was 0.001" or less which is far too low. I haven't yet started machining metal (my jobs are usually minor fab and in sheet metal), but I think I just tasted a key element in my education here, Pete. Thanks for sharing that. -- To see what is right, and not to do it, is want of courage or of principle. -- Confucius |
Better luck machining aluminum
"Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. -- Ed Huntress |
Better luck machining aluminum
On 2010-07-30, Ed Huntress wrote:
"Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i |
Better luck machining aluminum
"Ignoramus18915" wrote in message ... On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That's how it's generally done. If you can find some info on CNC moldmaking, you'll learn a lot about this kind of job. I haven't checked recently but some of the CAD and CAM companies have, in the past, had illustrated online descriptions of their pocketing, profiling, and contouring routines. If my old articles on the subject were still online, I could point you to a couple of them. g I covered the subject for _Machining_ and _Machine Shop Guide_. That's why I don't want to do CNC at home. It's too close to what I did for work. -- Ed Huntress |
Better luck machining aluminum
On 2010-07-30, Ed Huntress wrote:
"Ignoramus18915" wrote in message ... On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That's how it's generally done. If you can find some info on CNC moldmaking, you'll learn a lot about this kind of job. I haven't checked recently but some of the CAD and CAM companies have, in the past, had illustrated online descriptions of their pocketing, profiling, and contouring routines. If my old articles on the subject were still online, I could point you to a couple of them. g I covered the subject for _Machining_ and _Machine Shop Guide_. That's why I don't want to do CNC at home. It's too close to what I did for work. I do computer programming at home, and at work, I like it. No C++ at home though. i |
Better luck machining aluminum
Ignoramus18915 wrote: On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That follows the same concept of using a roughing mill and then a finish mill. If you ramp your regular end mill down in small Z steps, say 0.100" and are at your top 3,000 RPM, you can move at a much higher feed rate, say 30 IPM as a starting point. Your spindle RPM and the number of flutes on the end mill determines the feed rate that will give you a reasonable chip load. Your available HP determines how deep a cut you can take at that chip load. With your 2-3 HP available, I expect you can take deeper than 0.100" cuts with ease, but you probably want to limit it to 0.100" cuts to leave a smaller stairstep for your finish pass. This doesn't mean you can't optimize things with a roughing and finish pass with the regular end mill, using a much deeper cut for the initial bulk removal passes, and a 0.100" step for the final pass with the regular end mill. |
Better luck machining aluminum
On 2010-07-30, Pete C. wrote:
Ignoramus18915 wrote: On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That follows the same concept of using a roughing mill and then a finish mill. If you ramp your regular end mill down in small Z steps, say 0.100" and are at your top 3,000 RPM, you can move at a much higher feed rate, say 30 IPM as a starting point. I could even plunge on a helical curve along a circle, which is what I do. Your spindle RPM and the number of flutes on the end mill determines the feed rate that will give you a reasonable chip load. Your available HP determines how deep a cut you can take at that chip load. With your 2-3 HP available, I expect you can take deeper than 0.100" cuts with ease, but you probably want to limit it to 0.100" cuts to leave a smaller stairstep for your finish pass. This doesn't mean you can't optimize things with a roughing and finish pass with the regular end mill, using a much deeper cut for the initial bulk removal passes, and a 0.100" step for the final pass with the regular end mill. Got it. All good ideas. Thanks i |
Better luck machining aluminum
Ignoramus18915 wrote: On 2010-07-30, Pete C. wrote: Ignoramus18915 wrote: On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That follows the same concept of using a roughing mill and then a finish mill. If you ramp your regular end mill down in small Z steps, say 0.100" and are at your top 3,000 RPM, you can move at a much higher feed rate, say 30 IPM as a starting point. I could even plunge on a helical curve along a circle, which is what I do. That's pretty much what I meant by "ramp" vs. "step". Your spindle RPM and the number of flutes on the end mill determines the feed rate that will give you a reasonable chip load. Your available HP determines how deep a cut you can take at that chip load. With your 2-3 HP available, I expect you can take deeper than 0.100" cuts with ease, but you probably want to limit it to 0.100" cuts to leave a smaller stairstep for your finish pass. This doesn't mean you can't optimize things with a roughing and finish pass with the regular end mill, using a much deeper cut for the initial bulk removal passes, and a 0.100" step for the final pass with the regular end mill. Got it. All good ideas. Thanks i |
Better luck machining aluminum
"Ignoramus18915" wrote in message ... On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Ed Huntress wrote: "Ignoramus18915" wrote in message ... On 2010-07-30, Jon Elson wrote: Ignoramus5687 wrote: I have decided to dial way down this time. Again, I am making a mold cavity in aluminum for making a kids wax toy (toy railroad supports). This time I am using 1200 RPM and 1 IPM, and in addition I use WD-40. The good news is that nothing gums up, the bad news is that the speed is ridiculously slow. Yes, it is CNC, but still. Next thing on my list is getting coolant to work. I have a professional coolant tank with motor etc and also a little 1/70 HP pump that works great in plastic buckets. I think that I will use the latter Then I can go at the same 1200 RPM but at much higher feeds. I'm not sure coolant really helps pick up the feedrate. From the other thread it seems you are using a 3/8" endmill? I'd probably use 1800 RPM there, and for a 4-flute cutter I'd feed at about 10 IPM. And, much better to take lighter cuts and keep the cutter moving rather than taking a deep cut and crawling. At least, that's MY method. I think that part of my problem is that I use a ball endmill. I will mess more with it on the weekend. It can be difficult to get adequate surface speed near the center of a ball-nose cutter. It's tricky to program them for complex cuts, and plowing through solid metal with one is problematic. You usually use them to get the radius you need when you're cutting only on one side, and even then, you have to program speeds and feeds carefully so you aren't pushing the center of the ball at a rate faster than it will actually cut chips. Profiling is especially tricky. As for speeds, you can't run an ordinary mill at surface speeds in aluminum that are too fast for a carbide cutter. With a 3/8" endmill, you can't turn it too fast for HSS. And that's even running dry. Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. i That's how it's generally done. If you can find some info on CNC moldmaking, you'll learn a lot about this kind of job. I haven't checked recently but some of the CAD and CAM companies have, in the past, had illustrated online descriptions of their pocketing, profiling, and contouring routines. If my old articles on the subject were still online, I could point you to a couple of them. g I covered the subject for _Machining_ and _Machine Shop Guide_. That's why I don't want to do CNC at home. It's too close to what I did for work. I do computer programming at home, and at work, I like it. No C++ at home though. i My interest in machining as a hobby is mostly about the historical methods for achieving amazing things. If I wanted to sink a lot more money into a hobby, I might get into CNC. But I have a lot of fun making things to 0.0002" accuracy on antiques, using antique methods. I'm less interested in having finished products than I am in the processes of making things. I get off on clever faceplate work. d8-) -- Ed Huntress |
Better luck machining aluminum
On 2010-07-30, Ed Huntress wrote:
My interest in machining as a hobby is mostly about the historical methods for achieving amazing things. If I wanted to sink a lot more money into a hobby, I might get into CNC. But I have a lot of fun making things to 0.0002" accuracy on antiques, using antique methods. So far, not counting costs like renting a trailer, the whole shebang cost me $1,700. I'm less interested in having finished products than I am in the processes of making things. I get off on clever faceplate work. d8-) I like processes too. i |
Better luck machining aluminum
Ignoramus18915 wrote:
Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool to ball endmill and finish the sides and bottom. Yes, that is an excellent plan. There are also bull-nose end mills that have a radius at the tip, but a flat center. But, you never want to do roughing with a ball-end mill, due to the center not having any rotation. It is forced to "churn" the metal instead of cutting it. This is likely your problem, that churning causes both the work and tool to run extremely hot. The curved side of the ball-end mill can cut, but any contact with the center should be avoided. Jon |
Better luck machining aluminum
Ignoramus18915 wrote:
I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. Jon |
Better luck machining aluminum
On 2010-07-30, Jon Elson wrote:
Ignoramus18915 wrote: I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. I want to learn first what it is all about. But maybe later, yes. i |
Better luck machining aluminum
On 2010-07-30, Jon Elson wrote:
Ignoramus18915 wrote: Maybe I should change the whole program. I need to cut out a circular area of two nested cones: \__ __/ \___/ Maybe I should get a regular square end mill and mill out two circular pockets (wider on top and narrower on the bottom). Then change tool tod ball endmill and finish the sides and bottom. Yes, that is an excellent plan. There are also bull-nose end mills that have a radius at the tip, but a flat center. But, you never want to do roughing with a ball-end mill, due to the center not having any rotation. It is forced to "churn" the metal instead of cutting it. This is likely your problem, that churning causes both the work and tool to run extremely hot. The curved side of the ball-end mill can cut, but any contact with the center should be avoided. d Jon Yep, I am convinced. i |
Better luck machining aluminum
Ignoramus18915 wrote: On 2010-07-30, Jon Elson wrote: Ignoramus18915 wrote: I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. I want to learn first what it is all about. But maybe later, yes. i Definitely a good idea to fully understand the current code before hacking with it... |
Better luck machining aluminum
On 2010-07-30, Pete C. wrote:
Ignoramus18915 wrote: On 2010-07-30, Jon Elson wrote: Ignoramus18915 wrote: I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. I want to learn first what it is all about. But maybe later, yes. i Definitely a good idea to fully understand the current code before hacking with it... Yes. The machine is currently functional. Maybe not functioning at the top of its possible capacity and convenience (still have to do all those buttons, rigid tapping, look at the servo driven table for 4th axis, tune it better, etc etc). Despite that, I can already use it. As you can easily tell, I barely know anything about CNC, so there is much to learn. i |
Better luck machining aluminum
Ignoramus18915 wrote: On 2010-07-30, Pete C. wrote: Ignoramus18915 wrote: On 2010-07-30, Jon Elson wrote: Ignoramus18915 wrote: I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. I want to learn first what it is all about. But maybe later, yes. i Definitely a good idea to fully understand the current code before hacking with it... Yes. The machine is currently functional. Maybe not functioning at the top of its possible capacity and convenience (still have to do all those buttons, rigid tapping, look at the servo driven table for 4th axis, tune it better, etc etc). Despite that, I can already use it. As you can easily tell, I barely know anything about CNC, so there is much to learn. i See if you can find a copy of "Machining Fundamentals" ISBN 1-56637-662-9, it will give you a good foundation of the various machining processes. It covers some CNC, but the key thing to remember is that the CNC is doing basically the same thing as the manual, so the same machining principles apply. |
Better luck machining aluminum
On 2010-07-30, Pete C. wrote:
Ignoramus18915 wrote: On 2010-07-30, Pete C. wrote: Ignoramus18915 wrote: On 2010-07-30, Jon Elson wrote: Ignoramus18915 wrote: I do computer programming at home, and at work, I like it. No C++ at home though. Well, C++ is just one apt-get away! If you want to start tinkering with EMC2 components, you will need to install the C and C++ environment. I want to learn first what it is all about. But maybe later, yes. i Definitely a good idea to fully understand the current code before hacking with it... Yes. The machine is currently functional. Maybe not functioning at the top of its possible capacity and convenience (still have to do all those buttons, rigid tapping, look at the servo driven table for 4th axis, tune it better, etc etc). Despite that, I can already use it. As you can easily tell, I barely know anything about CNC, so there is much to learn. i See if you can find a copy of "Machining Fundamentals" ISBN 1-56637-662-9, it will give you a good foundation of the various machining processes. It covers some CNC, but the key thing to remember is that the CNC is doing basically the same thing as the manual, so the same machining principles apply. just bought it thanks i |
Better luck machining aluminum
Ignoramus18915 wrote:
Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. I've never used ball end end mills so I'm speculating here. Can you rough out the cavity with a conventional square end end mill? Since you piqued my interest about ball nose, I'm looking around a bit. Go read page 28-30+ http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf Also read: http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0 Do you know the difference between climb milling vs conventional? I prefer climb whenever the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a cnc it is the normal way since you don't have backlash to any degree compared to lead screws. Wes |
Better luck machining aluminum
On 2010-07-30, Wes wrote:
Ignoramus18915 wrote: Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. I've never used ball end end mills so I'm speculating here. Can you rough out the cavity with a conventional square end end mill? EXACTLY WHAT i WILL DO Since you piqued my interest about ball nose, I'm looking around a bit. Go read page 28-30+ http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf Very fun stuff. Also read: http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0 nice, just what i need Do you know the difference between climb milling vs conventional? I prefer climb whenever the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a cnc it is the normal way since you don't have backlash to any degree compared to lead screws. I am reworking everything nowto use climb. i |
Better luck machining aluminum
"Ignoramus18915" wrote in message ... On 2010-07-30, Wes wrote: Ignoramus18915 wrote: Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. I've never used ball end end mills so I'm speculating here. Can you rough out the cavity with a conventional square end end mill? EXACTLY WHAT i WILL DO Since you piqued my interest about ball nose, I'm looking around a bit. Go read page 28-30+ http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf Very fun stuff. Also read: http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0 nice, just what i need Do you know the difference between climb milling vs conventional? I prefer climb whenever the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a cnc it is the normal way since you don't have backlash to any degree compared to lead screws. I am reworking everything nowto use climb. You shouldn't have any trouble with it at all in aluminum. But pay close attention to how your machine behaves when climb-cutting in steel. In a small, conventional machine like yours, everything has to be tight or it will chatter or generate some other vibration. You'll know soon enough when you start using it. -- Ed Huntress |
Better luck machining aluminum
On 2010-07-30, Ed Huntress wrote:
"Ignoramus18915" wrote in message ... On 2010-07-30, Wes wrote: Ignoramus18915 wrote: Pete, I will try some more. The problem is, one mistake and the endmill snaps off. I think that I should practice with square end endmills instead of the ball ends. I have much more of those. I've never used ball end end mills so I'm speculating here. Can you rough out the cavity with a conventional square end end mill? EXACTLY WHAT i WILL DO Since you piqued my interest about ball nose, I'm looking around a bit. Go read page 28-30+ http://www.ingersoll.com/ictc/ictcpu...e/C-C580-3.pdf Very fun stuff. Also read: http://www.kennametal.com/images/pdf...PCFEVMCQFBYIV0 nice, just what i need Do you know the difference between climb milling vs conventional? I prefer climb whenever the machine can handle it. I usually climb mill on bridgeports with leadscrews and on a cnc it is the normal way since you don't have backlash to any degree compared to lead screws. I am reworking everything nowto use climb. You shouldn't have any trouble with it at all in aluminum. But pay close attention to how your machine behaves when climb-cutting in steel. In a small, conventional machine like yours, everything has to be tight or it will chatter or generate some other vibration. It weighs 5,000 lbs You'll know soon enough when you start using it. |
| All times are GMT +1. The time now is 05:03 PM. |
|
Powered by vBulletin® Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.
Copyright ©2004 - 2014 DIYbanter