|
What's a good endmill for cutting stainless plate? (encountering problems)
Hi, I'm currently making a thick flange on a CNC mill. The material is
a 1/2" thick plate of 321 stainless. Previously, we made a prototype out of 3/8" mild steel. That piece cut relatively easy, as was expected. We knew that the thicker stainless piece was going to be much tougher to cut, so we made sure that we used lower speeds and plenty of coolant. Here's the problem: Starting with a new Sossner 4 flute high speed steel endmill, the same kind that we used to cut the prototype, we began cutting the 321 stainless. The first 1/8 inch or so it was slow but steady, we expected it to be tough. But after that it began to chatter and the cutting slowed down. By about 1 inch of cutting, the endmill was worn out. Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? I know that people who work with stainless don't go through 30 endmills to make a relatively small piece. Does anyone have any recommendations of what kind of endmill to use to cut thick 321 stainless? Is the material that our endmill is composed of simply too soft a metal? Replacing cutters every couple of inches isn't an option. I'm sure that someone can lead me in the right direction. Thanks, Marshall |
What's a good endmill for cutting stainless plate? (encountering problems)
In article , Marshall Johnson
says... Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? Post up the sfpm you were running on the tool, and the feed rate. Either your idea of 'slow' for the rpm is incorrect, or you were running the feed rate so slow as to allow the material to work harden under the tool. Just a guess, there will be others here that will be more accurate. Jim ================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ================================================== |
What's a good endmill for cutting stainless plate? (encounteringproblems)
I have been milling a lot of 316 lately and have found that the main
thing you need is a lot of intestinal fortitude to crank up the feed rate. Especially on a middle weight mill like I have. You have to be pretty agressive to get under the surface that was work hardened on the previous rotation. Marshall Johnson wrote: Hi, I'm currently making a thick flange on a CNC mill. The material is a 1/2" thick plate of 321 stainless. Previously, we made a prototype out of 3/8" mild steel. That piece cut relatively easy, as was expected. We knew that the thicker stainless piece was going to be much tougher to cut, so we made sure that we used lower speeds and plenty of coolant. Here's the problem: Starting with a new Sossner 4 flute high speed steel endmill, the same kind that we used to cut the prototype, we began cutting the 321 stainless. The first 1/8 inch or so it was slow but steady, we expected it to be tough. But after that it began to chatter and the cutting slowed down. By about 1 inch of cutting, the endmill was worn out. Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? I know that people who work with stainless don't go through 30 endmills to make a relatively small piece. Does anyone have any recommendations of what kind of endmill to use to cut thick 321 stainless? Is the material that our endmill is composed of simply too soft a metal? Replacing cutters every couple of inches isn't an option. I'm sure that someone can lead me in the right direction. Thanks, Marshall -- Glenn Ashmore I'm building a 45' cutter in strip/composite. Watch my progress (or lack there of) at: http://www.rutuonline.com Shameless Commercial Division: http://www.spade-anchor-us.com |
What's a good endmill for cutting stainless plate? (encounteringproblems)
jim rozen wrote:
In article , Marshall Johnson says... Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? Post up the sfpm you were running on the tool, and the feed rate. Either your idea of 'slow' for the rpm is incorrect, or you were running the feed rate so slow as to allow the material to work harden under the tool. Just a guess, there will be others here that will be more accurate. Jim Besides rpm, endmill diameter, depth of cut, and conventional or climb milling should be considered. I like big roughers. wws |
What's a good endmill for cutting stainless plate? (encountering problems)
|
What's a good endmill for cutting stainless plate? (encountering problems)
Marshall,
I'm not familiar with 321, but with 316 the best cutter I have used is from M42. This is an chrome vanadium ISO alloy and it is high in cobalt (5%). Use a very slow speed, a high feed rate, lotsa coolant and small cuts. Take your time. Do not use a dull tool. As soon as the edge starts to fail, change immediately to prevent excessive work hardening. Steve "Marshall Johnson" wrote in message om... Hi, I'm currently making a thick flange on a CNC mill. The material is a 1/2" thick plate of 321 stainless. Previously, we made a prototype out of 3/8" mild steel. That piece cut relatively easy, as was expected. We knew that the thicker stainless piece was going to be much tougher to cut, so we made sure that we used lower speeds and plenty of coolant. Here's the problem: Starting with a new Sossner 4 flute high speed steel endmill, the same kind that we used to cut the prototype, we began cutting the 321 stainless. The first 1/8 inch or so it was slow but steady, we expected it to be tough. But after that it began to chatter and the cutting slowed down. By about 1 inch of cutting, the endmill was worn out. Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? I know that people who work with stainless don't go through 30 endmills to make a relatively small piece. Does anyone have any recommendations of what kind of endmill to use to cut thick 321 stainless? Is the material that our endmill is composed of simply too soft a metal? Replacing cutters every couple of inches isn't an option. I'm sure that someone can lead me in the right direction. Thanks, Marshall |
What's a good endmill for cutting stainless plate? (encountering problems)
jim rozen wrote in message ...
Post up the sfpm you were running on the tool, and the feed rate. Either your idea of 'slow' for the rpm is incorrect, or you were running the feed rate so slow as to allow the material to work harden under the tool. Sorry for the late reply. The spindle speed was 200 rpm. Originally the feed rate was 1.5" per minute, but that was when we wrote the program for the mild steel. By the time we were taking a good cut into the metal, we had the feed rate slowed down to about 1/10" an inch per minute. Keep in mind that we were trying to cut through this 1/2" piece in one pass. It looks like we're going to have to bump up the feed rate and only go half way through the piece on each pass, or maybe even less. |
What's a good endmill for cutting stainless plate? (encountering problems)
In article , Marshall Johnson
says... The spindle speed was 200 rpm. Ok, that's only *part* of the number you need. How large is the end mill diameter? From that you can calculate the *surface* feet per minute that the cutting tool is running at. That's what counts. Jim ================================================== please reply to: JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com ================================================== |
What's a good endmill for cutting stainless plate? (encounteringproblems)
Marshall Johnson wrote: jim rozen wrote in message ... Post up the sfpm you were running on the tool, and the feed rate. Either your idea of 'slow' for the rpm is incorrect, or you were running the feed rate so slow as to allow the material to work harden under the tool. Sorry for the late reply. The spindle speed was 200 rpm. Originally the feed rate was 1.5" per minute, but that was when we wrote the program for the mild steel. By the time we were taking a good cut into the metal, we had the feed rate slowed down to about 1/10" an inch per minute. Well, there's your problem! With any material that work hardens (SS is notorious for this, but many other harder materials also do it) you reduce the depth of cut, and may need to INCREASE the feedrate! There's no way you can make this cut in a single pass except with monster machines and very large diameter cutters. (A horizontal mill could do it in one pass if rigid enough, but due to the nature of the cutting action, a vertical mill ends up producing very thin chips at the sides when plowing at full width, and this is where the work hardening begins to develop.) Jon Keep in mind that we were trying to cut through this 1/2" piece in one pass. It looks like we're going to have to bump up the feed rate and only go half way through the piece on each pass, or maybe even less. |
What's a good endmill for cutting stainless plate? (encountering problems)
replying to Marshall Johnson, WTF STEEL wrote:
Marshallj25 wrote: Hi, I'm currently making a thick flange on a CNC mill. The material is a 1/2" thick plate of 321 stainless. Previously, we made a prototype out of 3/8" mild steel. That piece cut relatively easy, as was expected. We knew that the thicker stainless piece was going to be much tougher to cut, so we made sure that we used lower speeds and plenty of coolant. Here's the problem: Starting with a new Sossner 4 flute high speed steel endmill, the same kind that we used to cut the prototype, we began cutting the 321 stainless. The first 1/8 inch or so it was slow but steady, we expected it to be tough. But after that it began to chatter and the cutting slowed down. By about 1 inch of cutting, the endmill was worn out. Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? I know that people who work with stainless don't go through 30 endmills to make a relatively small piece. Does anyone have any recommendations of what kind of endmill to use to cut thick 321 stainless? Is the material that our endmill is composed of simply too soft a metal? Replacing cutters every couple of inches isn't an option. I'm sure that someone can lead me in the right direction. Thanks, Marshall sadly you will have to cut a few inches and replace cutter because the 321 stainless is to tough for it to work -- posted from http://www.polytechforum.com/metalwo...te-298349-.htm using PolytechForum's Web, RSS and Social Media Interface to rec.crafts.metalworking and other engineering groups |
What's a good endmill for cutting stainless plate? (encountering problems)
WTF STEEL wrote:
replying to Marshall Johnson, WTF STEEL wrote: Marshallj25 wrote: Hi, I'm currently making a thick flange on a CNC mill. The material is a 1/2" thick plate of 321 stainless. Previously, we made a prototype out of 3/8" mild steel. That piece cut relatively easy, as was expected. We knew that the thicker stainless piece was going to be much tougher to cut, so we made sure that we used lower speeds and plenty of coolant. Here's the problem: Starting with a new Sossner 4 flute high speed steel endmill, the same kind that we used to cut the prototype, we began cutting the 321 stainless. The first 1/8 inch or so it was slow but steady, we expected it to be tough. But after that it began to chatter and the cutting slowed down. By about 1 inch of cutting, the endmill was worn out. Something's not right here. I knew it would be tough but not THAT tough. How come the endmill wore out so quickly? I know that people who work with stainless don't go through 30 endmills to make a relatively small piece. Does anyone have any recommendations of what kind of endmill to use to cut thick 321 stainless? Is the material that our endmill is composed of simply too soft a metal? Replacing cutters every couple of inches isn't an option. I'm sure that someone can lead me in the right direction. Thanks, Marshall sadly you will have to cut a few inches and replace cutter because the 321 stainless is to tough for it to work Bull**** . They make solid carbide end mills just for such tough materials .. Cobalt EM's too might do the job , I haven't tried mine on that particular alloy but it worked well on some 4140 I cut recently - I'd go with at least 3/8 or 1/2 inch , low rotation speed and fairly heavy feed with plenty of coolant . -- Snag --- This email is free from viruses and malware because avast! Antivirus protection is active. http://www.avast.com |
What's a good endmill for cutting stainless plate? (encountering problems)
In article ,
"Snag" wrote: They make solid carbide end mills just for such tough materials . Cobalt EM's too might do the job , I haven't tried mine on that particular alloy but it worked well on some 4140 I cut recently - I'd go with at least 3/8 or 1/2 inch , low rotation speed and fairly heavy feed with plenty of coolant . Aaaand the fundamental difference (which leads to Snag correctly recommending slow rotation and heavy feed) is that unlike mild steel, stainless work hardens very significantly. If you "take it easy" and cut fine shavings you will fail 10 times out of 10. You have to cut serious chips or not at all. It can be hard to wrap your head around, since the instinctive response is to back off and go easy since it cuts hard - that just happens to be exactly wrong for stainless. Each new cut needs to get "beneath/beyond" the work-hardened "crust" of the previous cut. Lubrication was not mentioned - use some. -- Cats, coffee, chocolate...vices to live by Please don't feed the trolls. Killfile and ignore them so they will go away. |
What's a good endmill for cutting stainless plate? (encountering problems)
Just out of curiosity, now that the OP has work hardened the part, how does
he get going again? Will the solid carbide cutter do it? Pete Stanaitis ---------------- |
What's a good endmill for cutting stainless plate? (encountering problems)
Pete S wrote:
Just out of curiosity, now that the OP has work hardened the part, how does he get going again? Will the solid carbide cutter do it? Pete Stanaitis ---------------- If it does like 4140 that hard area will only be a skin a few thou thick . If he can get under that skin it should be OK - and yes , carbide will cut it . So will diamond ... I have a handful of diamond router bits , they were too dull to cut particle board/MDF at 35,000 RPM but they do a swell job for light cuts at lower speeds in very hard materials . They don't like interrupted cuts ... -- Snag --- This email is free from viruses and malware because avast! Antivirus protection is active. http://www.avast.com |
| All times are GMT +1. The time now is 04:24 PM. |
Powered by vBulletin® Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.
Copyright ©2004 - 2014 DIYbanter