I'm new to high speed machining. I'm cutting a brass part
http://i1262.photobucket.com/albums/...63/Chatter.jpg
with a 4mm HSS Co TICN cutter. The surfacing works fine, but when I try to make a deep counterbore I get a really bad finish. I'm running the tool at 10k rpm (spindle range is 8k-25k rpm) and the finishing pass at F300. I'm not sure what my F values actually mean, like in ipm, but it looks like a good speed. I suppose my my options are to use a carbide cutter, go to 6mm diameter (max on this spindle), or adjust the feedrate and spindle speed. Can anyone take a look and make suggestions? I know I should get myself a proper knee mill, but that's not a realistic option for me at the moment. I'm hoping the machine I have
http://i1262.photobucket.com/albums/...r1963/CNC1.jpg
will be adequate if I tweak the operation enough.

"robobass" wrote in message
...
I'm new to high speed machining. I'm cutting a brass part
http://i1262.photobucket.com/albums/...63/Chatter.jpg
with a 4mm HSS Co TICN cutter. The surfacing works fine, but when I
try to make a deep counterbore I get a really bad finish. I'm running
the tool at 10k rpm (spindle range is 8k-25k rpm) and the finishing
pass at F300. I'm not sure what my F values actually mean, like in
ipm, but it looks like a good speed. I suppose my my options are to
use a carbide cutter, go to 6mm diameter (max on this spindle), or
adjust the feedrate and spindle speed. Can anyone take a look and make
suggestions? I know I should get myself a proper knee mill, but that's
not a realistic option for me at the moment. I'm hoping the machine I
have
http://i1262.photobucket.com/albums/...r1963/CNC1.jpg
will be adequate if I tweak the operation enough.

===========================

I suspect you won't like what you see if you put an indicator on the
head to measure deflection and pull on it with a spring scale.

I got a chainsaw finish from milling meter cutouts in 0.030" sheet
Aluminum with a 1/4" end mill with flutes 2" long, which I was using
to clear a forest of clamps. The reason was tool flex, not the
machine; a 1/2" diameter cutter gave a smooth finish at the cost of
more filing to square the corners.

My 700 Lb Clausing's spindle deflects ~0.001" per 25 Lbs.

-jsw

On Fri, 13 Feb 2015 01:36:10 -0800 (PST), robobass
wrote:

I'm new to high speed machining. I'm cutting a brass part
http://i1262.photobucket.com/albums/...63/Chatter.jpg
with a 4mm HSS Co TICN cutter. The surfacing works fine, but when I try to make a deep counterbore I get a really bad finish. I'm running the tool at 10k rpm (spindle range is 8k-25k rpm) and the finishing pass at F300. I'm not sure what my F values actually mean, like in ipm, but it looks like a good speed. I suppose my my options are to use a carbide cutter, go to 6mm diameter (max on this spindle), or adjust the feedrate and spindle speed. Can anyone take a look and make suggestions? I know I should get myself a proper knee mill, but that's not a realistic option for me at the moment. I'm hoping the machine I have
http://i1262.photobucket.com/albums/...r1963/CNC1.jpg
will be adequate if I tweak the operation enough.

Brass likes to grab cutters -- they dig in if they have any positive
rake at all. Zero rake or slight negative rake may solve your problem.
On a lathe tool, that's easy. On a milling cutter, your options are
limited. You can try dubbing off the very edges of the cutter with a
small stone.

First try just giving it a little radius -- really small. If that
doesn't do it, try honing a slight negative angle on the very edge. At
those rpm, you don't have to hone more than a couple of thousanths
back from the edge, because you aren't cutting deep to begin with.

Your machine and the coarseness of the chatter suggests, however, that
any "digging in" is being amplified by a lack of rigidity in the whole
setup. That's going to make it tricky.

Anyway, this is a cheap and easy thing to try first.

Cute kid, BTW.

--
Ed Huntress

What is the make of the spindle on your machine? I've been looking for one
of that size.

Hul

robobass wrote:
I'm new to high speed machining. I'm cutting a brass part
http://i1262.photobucket.com/albums/...63/Chatter.jpg
with a 4mm HSS Co TICN cutter. The surfacing works fine, but when I try to make a deep counterbore I get a really bad finish. I'm running the tool at 10k rpm (spindle range is 8k-25k rpm) and the finishing pass at F300. I'm not sure what my F values actually mean, like in ipm, but it looks like a good speed. I suppose my my options are to use a carbide cutter, go to 6mm diameter (max on this spindle), or adjust the feedrate and spindle speed. Can anyone take a look and make suggestions? I know I should get myself a proper knee mill, but that's not a realistic option for me at the moment. I'm hoping the machine I have
http://i1262.photobucket.com/albums/...r1963/CNC1.jpg
will be adequate if I tweak the operation enough.

On Friday, February 13, 2015 at 11:58:50 PM UTC+1, Hul Tytus wrote:
What is the make of the spindle on your machine? I've been looking for one
of that size.

Hul

Sorry, I have zero documentation on the motor, and there isn't any sort of label anywhere on it. I bought the machine from a Russian guy who was very helpful walking me through the Mach3 configuration and even threw in an XP desktop fully set up. He was, however, a bit evasive on the origin of the components. He is a serious mold maker, has two similar machines in his own shop with the same parts as mine, but he uses a Bridgeport for brass.

I just ordered two 6mm carbide cutters. Maybe I'll try grinding the flutes on one of them. I did notice that my 3mm carbide mill cuts brass with way less effort than the HSS Co. Maybe the combination of carbide and a larger radius will be enough. Two finishing passes too? I don't need a mirror finish, but it's gotta be better than it is now!
Thanks everyone.

On Sat, 14 Feb 2015 04:15:43 -0800 (PST), robobass
wrote:

I just ordered two 6mm carbide cutters. Maybe I'll try grinding the flutes on one of them. I did notice that my 3mm carbide mill cuts brass with way less effort than the HSS Co. Maybe the combination of carbide and a larger radius will be enough. Two finishing passes too? I don't need a mirror finish, but it's gotta be better than it is now!
Thanks everyone.

Something is funny there. There should be little or no difference in
the "effort" required by a carbide cutter versus HSS. If anything, the
HSS should require slightly less effort, given equal sharpness.

The only reason to go with carbide when cutting brass is if you're
burning your HSS cutters. This is extremely unlikely.

There is one other potential issue, however: Carbide is stiffer. If
the flexibility of the cutter itself is contributing to the chatter,
carbide could help.

--
Ed Huntress

On Saturday, February 14, 2015 at 7:08:42 AM UTC-5, robobass wrote in rec.crafts.metalworking:
On Friday, February 13, 2015 at 11:58:50 PM UTC+1, Hul Tytus wrote in
rec.crafts.metalworking:
What is the make of the spindle on your machine? I've been looking for one
of that size.

Sorry, I have zero documentation on the motor, and there isn't any sort
of label anywhere on it. I bought the machine from a Russian guy who
was very helpful walking me through the Mach3 configuration and even
threw in an XP desktop fully set up. He was, however, a bit evasive
on the origin of the components.

Not to change the subject, but I've noticed that with amateur phone repairmen/salesmen. I was running around trying to get my phone working again BEFORE I thought of typing in the symptoms that the phone was having into a search engine. All I heard was "go see someone else" or something similar or buy a new phone.

So, when I finally typed my phone's trouble into a search engine: I noticed on various website discussions that others were having the same difficulty with the same model and I tried their solutions and it worked.

Sometimes, DIY is better than what's out there.

Something is funny there. There should be little or no difference in
the "effort" required by a carbide cutter versus HSS. If anything, the
HSS should require slightly less effort, given equal sharpness.

The only reason to go with carbide when cutting brass is if you're
burning your HSS cutters. This is extremely unlikely.

There is one other potential issue, however: Carbide is stiffer. If
the flexibility of the cutter itself is contributing to the chatter,
carbide could help.

--
Ed Huntress

The tool has 22mm of 4mm length, so I'm thinking deflection is a suspect, and a shorter (and carbide) tool should help. As far as carbide vs. HSSE, so far I've noticed that it plunges with much less strain, but I haven't used it enough for profiling to draw a conclusion.

On Saturday, February 14, 2015 at 5:24:21 PM UTC+1, wrote:
On Saturday, February 14, 2015 at 7:08:42 AM UTC-5, robobass wrote in rec..crafts.metalworking:
On Friday, February 13, 2015 at 11:58:50 PM UTC+1, Hul Tytus wrote in
rec.crafts.metalworking:
What is the make of the spindle on your machine? I've been looking for one
of that size.

Sorry, I have zero documentation on the motor, and there isn't any sort
of label anywhere on it. I bought the machine from a Russian guy who
was very helpful walking me through the Mach3 configuration and even
threw in an XP desktop fully set up. He was, however, a bit evasive
on the origin of the components.

Not to change the subject, but I've noticed that with amateur phone repairmen/salesmen. I was running around trying to get my phone working again BEFORE I thought of typing in the symptoms that the phone was having into a search engine. All I heard was "go see someone else" or something similar or buy a new phone.

So, when I finally typed my phone's trouble into a search engine: I noticed on various website discussions that others were having the same difficulty with the same model and I tried their solutions and it worked.

Sometimes, DIY is better than what's out there.

I have been searching the google, but haven't found anything specific enough. Sorry if I'm boring you, but isn't this a nice break from all the ATF stuff?

On Sat, 14 Feb 2015 08:40:19 -0800 (PST), robobass
wrote:


Something is funny there. There should be little or no difference in
the "effort" required by a carbide cutter versus HSS. If anything, the
HSS should require slightly less effort, given equal sharpness.

The only reason to go with carbide when cutting brass is if you're
burning your HSS cutters. This is extremely unlikely.

There is one other potential issue, however: Carbide is stiffer. If
the flexibility of the cutter itself is contributing to the chatter,
carbide could help.

--
Ed Huntress

The tool has 22mm of 4mm length, so I'm thinking deflection is a suspect, and a shorter (and carbide) tool should help. As far as carbide vs. HSSE, so far I've noticed that it plunges with much less strain, but I haven't used it enough for profiling to draw a conclusion.

There are several things that could be going on here, and I don't like
to speculate too much -- especialy from a still photo -- but here are
a couple of thoughts that may help.

First, if there's a difference in plunging with carbide versus HSS,
it's due to geometry or edge sharpness, not the tool material. It's
difficult to make any carbide as sharp as HSS but the carbide may be
sharper to begin with.

Second, 22 mm extension on a 4 mm cutter is indeed an invitation to
deflection and initiating vibration. Carbide is much stiffer.

Third, the machine configuration looks like an invitation to
sympathetic vibrations; changing speeds could help deal with any
oscillations. Have you tried slowing it down? That's why they build
machine tools from cast iron. It doesn't like to vibrate. g

Regarding dubbing, radiusing, or back-chamferring the cutting edge: it
could solve any digging-in, to which brass is very prone; or, by
increasing the cutting force, a radiused or negative-chamferred edge
could make things worse, by increasing tool deflection.

Chatter can be difficult to track down. Good luck.

--
Ed Huntress

On Saturday, February 14, 2015 at 6:03:26 PM UTC+1, Ed Huntress wrote:
On Sat, 14 Feb 2015 08:40:19 -0800 (PST), robobass
wrote:


Something is funny there. There should be little or no difference in
the "effort" required by a carbide cutter versus HSS. If anything, the
HSS should require slightly less effort, given equal sharpness.

The only reason to go with carbide when cutting brass is if you're
burning your HSS cutters. This is extremely unlikely.

There is one other potential issue, however: Carbide is stiffer. If
the flexibility of the cutter itself is contributing to the chatter,
carbide could help.

--
Ed Huntress

The tool has 22mm of 4mm length, so I'm thinking deflection is a suspect, and a shorter (and carbide) tool should help. As far as carbide vs. HSSE, so far I've noticed that it plunges with much less strain, but I haven't used it enough for profiling to draw a conclusion.

There are several things that could be going on here, and I don't like
to speculate too much -- especialy from a still photo -- but here are
a couple of thoughts that may help.

First, if there's a difference in plunging with carbide versus HSS,
it's due to geometry or edge sharpness, not the tool material. It's
difficult to make any carbide as sharp as HSS but the carbide may be
sharper to begin with.

Second, 22 mm extension on a 4 mm cutter is indeed an invitation to
deflection and initiating vibration. Carbide is much stiffer.

Third, the machine configuration looks like an invitation to
sympathetic vibrations; changing speeds could help deal with any
oscillations. Have you tried slowing it down? That's why they build
machine tools from cast iron. It doesn't like to vibrate. g

Regarding dubbing, radiusing, or back-chamferring the cutting edge: it
could solve any digging-in, to which brass is very prone; or, by
increasing the cutting force, a radiused or negative-chamferred edge
could make things worse, by increasing tool deflection.

Chatter can be difficult to track down. Good luck.

--
Ed Huntress

"the machine configuration looks like an invitation to
sympathetic vibrations"
Yeah. That too. The table definitely moves around alot, so I'm at the moment working on securing it to the brick walls.

On Fri, 13 Feb 2015 07:26:30 -0500, "Jim Wilkins"
wrote:

"robobass" wrote in message
...
I'm new to high speed machining. I'm cutting a brass part
http://i1262.photobucket.com/albums/...63/Chatter.jpg
with a 4mm HSS Co TICN cutter. The surfacing works fine, but when I
try to make a deep counterbore I get a really bad finish. I'm running
the tool at 10k rpm (spindle range is 8k-25k rpm) and the finishing
pass at F300. I'm not sure what my F values actually mean, like in
ipm, but it looks like a good speed. I suppose my my options are to
use a carbide cutter, go to 6mm diameter (max on this spindle), or
adjust the feedrate and spindle speed. Can anyone take a look and make
suggestions? I know I should get myself a proper knee mill, but that's
not a realistic option for me at the moment. I'm hoping the machine I
have
http://i1262.photobucket.com/albums/...r1963/CNC1.jpg
will be adequate if I tweak the operation enough.

===========================

I suspect you won't like what you see if you put an indicator on the
head to measure deflection and pull on it with a spring scale.

I got a chainsaw finish from milling meter cutouts in 0.030" sheet
Aluminum with a 1/4" end mill with flutes 2" long, which I was using
to clear a forest of clamps. The reason was tool flex, not the
machine; a 1/2" diameter cutter gave a smooth finish at the cost of
more filing to square the corners.

My 700 Lb Clausing's spindle deflects ~0.001" per 25 Lbs.

-jsw


Ill have to agree. And I dont see if he is using a 2 flute or 4 flute
cutter..and in his case..its going to need to be a 2 flute. Slow the
feed rate way the frack down..something like 10-30 IMP would be
pushing it, partciularly with a single deep cut. Brass is brittle,
not real ductile like aluminum..but its still ductile and will load up
your endmill and plug that sucker up trying to unload chips. And of
course he is cutting it dry..which at those speeds..he should be at
the very least..using a mist coolant..not so much for cooling..but for
lubrication of the chips.

Gunner

"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

On 2/14/2015 6:23 AM, Ed Huntress wrote:
On Sat, 14 Feb 2015 04:15:43 -0800 (PST), robobass
wrote:

I just ordered two 6mm carbide cutters. Maybe I'll try grinding the flutes on one of them. I did notice that my 3mm carbide mill cuts brass with way less effort than the HSS Co. Maybe the combination of carbide and a larger radius will be enough. Two finishing passes too? I don't need a mirror finish, but it's gotta be better than it is now!
Thanks everyone.

Something is funny there. There should be little or no difference in
the "effort" required by a carbide cutter versus HSS. If anything, the
HSS should require slightly less effort, given equal sharpness.

The only reason to go with carbide when cutting brass is if you're
burning your HSS cutters. This is extremely unlikely.

There is one other potential issue, however: Carbide is stiffer. If
the flexibility of the cutter itself is contributing to the chatter,
carbide could help.

Right and if the cutter is a 4 flute, there isn't time for cuttings to
clear before the next tooth comes and that might be the jitter. Turn
slower and move slower and see if the roughness goes away.

HSS really HSS not 'cheap steel' cutters would be far above a match
and can have a sharp edge to shave off the brass cleanly.

The nose on carbide is rounded as carbide shatters easily if pointed.

I use carbide on Bronze and HSS on brass. I mill and turn both.

Another issue might be to deep of a slot being cut. Hogging out to much
metal in a pass.

Martin

Ill have to agree. And I dont see if he is using a 2 flute or 4 flute
cutter..and in his case..its going to need to be a 2 flute. Slow the
feed rate way the frack down..something like 10-30 IMP would be
pushing it, partciularly with a single deep cut. Brass is brittle,
not real ductile like aluminum..but its still ductile and will load up
your endmill and plug that sucker up trying to unload chips. And of
course he is cutting it dry..which at those speeds..he should be at
the very least..using a mist coolant..not so much for cooling..but for
lubrication of the chips.

Gunner

More detail: Two flute Hss-Co-TICN, roughing with 2mm depths and 1mm stepover, .3mm finishing pass at full depth.

I don't think I need coolant. The chips fly far away and the cutting area stays clear and cool.

It's been suggested that I make the finishing pass .05mm and raise the tool .05mm so it isn't touching the bottom. I still think a big issue is the tool being so long and skinny. Haven't had a chance yet to run a thicker, shorter tool.

On Mon, 16 Feb 2015 03:09:13 -0800 (PST),
wrote:



Ill have to agree. And I dont see if he is using a 2 flute or 4 flute
cutter..and in his case..its going to need to be a 2 flute. Slow the
feed rate way the frack down..something like 10-30 IMP would be
pushing it, partciularly with a single deep cut. Brass is brittle,
not real ductile like aluminum..but its still ductile and will load up
your endmill and plug that sucker up trying to unload chips. And of
course he is cutting it dry..which at those speeds..he should be at
the very least..using a mist coolant..not so much for cooling..but for
lubrication of the chips.

Gunner

More detail: Two flute Hss-Co-TICN, roughing with 2mm depths and 1mm stepover, .3mm finishing pass at full depth.

I don't think I need coolant. The chips fly far away and the cutting area stays clear and cool.

It's been suggested that I make the finishing pass .05mm and raise the tool .05mm so it isn't touching the bottom. I still think a big issue is the tool being so long and skinny. Haven't had a chance yet to run a thicker, shorter tool.

Long skinny tools should ALWAYS make shallow cuts on each pass.


"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

Long skinny tools should ALWAYS make shallow cuts on each pass.

I feel like I'm doing that. Should I reduce the passes even more?

On Wed, 18 Feb 2015 00:12:32 -0800 (PST), robobass
wrote:


Long skinny tools should ALWAYS make shallow cuts on each pass.

I feel like I'm doing that. Should I reduce the passes even more?

Generally..and Im speaking as someone who only keeps the machines
running and only dabbles at machining....diameter of the mill = depth
of cut.

with "average" hobby machines for hobbyists in aluminum. Double the
depth if you can run over 3000 rpm. Not a "truth"..just a suggestion.

Got an 1/8" endmill..never cut more than 1/8" deep per pass
3/8" endmill...never more than 3/8" etc etc.

This of course may change a bit if you are using coolant with flood,
or with mist etc etc etc.

I would Strongly recommend using a machinest's calculator and then
making notes if your machine isnt rigid or fast enough...and a
plastics/wood router..is NOT rigid by any means. My mill weighs 2700
lbs. Its rigid.

http://hsmadvisor.com/index.php?page=Download

Cutting metals..is not like cutting wood and plastic

There are quite a number of similar Free programs out there..some of
which are designed to run on your smart phone..if you dont have a
computer out in the shop. Some are good, some are crappy..some are
very good. Most of the very good ones will cost you money. Not
all..but most.

Im sure folks here will suggest various programs or even give you the
formulas or an online calculator.

I use my android cellphone as a speeds and feeds calculator.

https://play.google.com/store/apps/d...lculator&hl=en

http://www.cnczone.com/forums/news-a...id-phones.html

try this one on your computer

http://zero-divide.net/?page=fswizard

Try this one on your Android phone..if you have one

https://play.google.com/store/apps/d....fswizard_lite


"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

Update. I did a bunch of things. Got a beefier vise, added more fasteners on the table, reduced the finishing pass width, depth and feedrate, and went with a thicker and shorter carbide mill (instead of HSS-Co) for the finish.. Result is Super. You would never know I did the work on a gantry router instead of a knee mill!

On Tue, 24 Feb 2015 07:40:57 -0800 (PST), robobass
wrote:

Update. I did a bunch of things. Got a beefier vise, added more fasteners on the table, reduced the finishing pass width, depth and feedrate, and went with a thicker and shorter carbide mill (instead of HSS-Co) for the finish. Result is Super. You would never know I did the work on a gantry router instead of a knee mill!

Great news! You'll never know which change(s) did it, but it's still
good.

--
Ed Huntress

On Tuesday, February 24, 2015 at 7:41:00 AM UTC-8, robobass wrote:
Update. I did a bunch of things. Got a beefier vise, added more fasteners on the table, reduced the finishing pass width, depth and feedrate, and went with a thicker and shorter carbide mill (instead of HSS-Co) for the finish. Result is Super. You would never know I did the work on a gantry router instead of a knee mill!

Real Estate: location, location, location.

Machining: rigidity, rigidity, rigidity

On Tue, 24 Feb 2015 07:40:57 -0800 (PST), robobass
wrote:

Update. I did a bunch of things. Got a beefier vise, added more fasteners on the table, reduced the finishing pass width, depth and feedrate, and went with a thicker and shorter carbide mill (instead of HSS-Co) for the finish.
Result is Super. You would never know I did the work on a gantry router instead of a knee mill!

Doesnt it feel good to do it the right way?

(VBG)



"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

Doesnt it feel good to do it the right way?

(VBG)

OH Yeah Baby!

On Tuesday, February 24, 2015 at 3:10:45 PM UTC-5, jon_banquer wrote:
On Tuesday, February 24, 2015 at 7:41:00 AM UTC-8, robobass wrote:
Update. I did a bunch of things. Got a beefier vise, added more fasteners on the table, reduced the finishing pass width, depth and feedrate, and went with a thicker and shorter carbide mill (instead of HSS-Co) for the finish. Result is Super. You would never know I did the work on a gantry router instead of a knee mill!


Real Estate: location, location, location.

That and I guess, make sure you've bought before national unemployment gets below 5%.

On Tuesday, February 24, 2015 at 11:29:02 PM UTC-8, robobass wrote:
Doesnt it feel good to do it the right way?

(VBG)

OH Yeah Baby!

When you have rigidity most of your problem go away or are much easier to diagnose.

On Wednesday, February 25, 2015 at 6:25:20 PM UTC+1, jon_banquer wrote:
On Tuesday, February 24, 2015 at 11:29:02 PM UTC-8, robobass wrote:
Doesnt it feel good to do it the right way?

(VBG)

OH Yeah Baby!

When you have rigidity most of your problem go away or are much easier to diagnose.

Well, you only get so much rigidity with a machine like this. You have to learn to work around it. Now I've discovered that the MDF table is not exactly on the X-Y plane of the spindle. Surprise!. I didn't discover this until I ran an array of 24 parts. It wasn't off enough do destroy the job, but I can easily correct it by facing the mounting plate before I make the next run. Yes, it's not a knee mill, but with care and tweaking I can cut brass. I paid 3.5K for a fully set up CNC with about 25" x 30" x 5" XYZ travel, and I don't need riggers to move it. Works for me. I don't need to cut steel though.

On Wednesday, February 25, 2015 at 12:30:48 PM UTC-8, robobass wrote:
On Wednesday, February 25, 2015 at 6:25:20 PM UTC+1, jon_banquer wrote:
On Tuesday, February 24, 2015 at 11:29:02 PM UTC-8, robobass wrote:
Doesnt it feel good to do it the right way?

(VBG)

OH Yeah Baby!

When you have rigidity most of your problem go away or are much easier to diagnose.

Well, you only get so much rigidity with a machine like this. You have to learn to work around it. Now I've discovered that the MDF table is not exactly on the X-Y plane of the spindle. Surprise!. I didn't discover this until I ran an array of 24 parts. It wasn't off enough do destroy the job, but I can easily correct it by facing the mounting plate before I make the next run. Yes, it's not a knee mill, but with care and tweaking I can cut brass. I paid 3.5K for a fully set up CNC with about 25" x 30" x 5" XYZ travel, and I don't need riggers to move it. Works for me. I don't need to cut steel though.

I think you mean your spindle axis(Z)is not perpendicular to the XY plane (your table), right?

A knee mill, such as a Bridgeport Series I, isn't very rigid as the table hangs over the saddle and is unsupported. The advantage of a Bridgeport type knee mill is that it's very versatile at the expense of rigidity. Bridgeport series I knee mills also suffer from a knuckle that isn't very rigid at the expense of versatility (The head can be tilted left or right as well as front to back).

Do you have a link to the CNC machine you own?

On Wed, 25 Feb 2015 12:30:47 -0800 (PST), robobass
wrote:

On Wednesday, February 25, 2015 at 6:25:20 PM UTC+1, jon_banquer wrote:
On Tuesday, February 24, 2015 at 11:29:02 PM UTC-8, robobass wrote:
Doesnt it feel good to do it the right way?

(VBG)

OH Yeah Baby!

When you have rigidity most of your problem go away or are much easier to diagnose.

Well, you only get so much rigidity with a machine like this. You have to learn to work around it. Now I've discovered that the MDF table is not exactly on the X-Y plane of the spindle. Surprise!. I didn't discover this until I ran an array of 24 parts. It wasn't off enough do destroy the job, but I can easily correct it by facing the mounting plate before I make the next run. Yes, it's not a knee mill, but with care and tweaking I can cut brass. I paid 3.5K for a fully set up CNC with about 25" x 30" x 5" XYZ travel, and I don't need riggers to move it. Works for me. I don't need to cut steel though.

Is the MDF not level (it actually is pretty good stuff) or is the
machine not plumb? Note..that the farther out from an unlevel machine
you go..the worse the alignment gets. So align your machine
first!...then worry about the table tops flatness. MDF is pretty good
stuff for this sort of work. Its usually within .001-.002 or less.
Ive used some that was .0005. Damned near as level as a surface plate.

Gunner

"At the core of liberalism is the spoiled child,
miserable, as all spoiled children are, unsatisfied,
demanding, ill-disciplined, despotic and useless.
Liberalism is a philosophy of sniveling brats."
PJ O'Rourke

"I think you mean your spindle axis(Z)is not perpendicular to the XY plane (your table), right?"

Yes. I made sure the spindle was perpendicular to the carriage, but the entire transport assembly appears to not be fully aligned to the table base. The only way I can see to adjust it is with shims, or to face the whole table.

Here is the machine:

http://s1262.photobucket.com/user/Mo...slideshow/CNC2

If you look at the first photo, you see that the table seems to dip toward the lower left. It could also be that I just mounted the work poorly, among other things. The quick fix is to simply face the plastic block before the next run. Something I should have done first, but the block itself seemed pretty good.

"Do you have a link to the CNC machine you own?"

No. It seems to be hand built by the seller. There is "RT Technik" engraved on the front, but I found no web hits. Few of the components even have labels, but the seller says he got everything locally, and to contact him if I need any parts. Here in Germany there are maybe a dozen commercial manufacturers building machines like this, as well as many individuals making them in their garages and selling them on Ebay. I shopped for a year and this is what I chose. So far it seems like I did well. Much of the Mach3 controller software is still a mystery to me, but fortunately the seller walked me through the basics. The hardest part has been creating decent toolpaths using Bobcad26. I'm not sure that was a good decision, but I am getting the job done now, after like two months of despair.

On Thursday, February 26, 2015 at 12:53:33 AM UTC-8, robobass wrote:
"I think you mean your spindle axis(Z)is not perpendicular to the XY plane (your table), right?"

Yes. I made sure the spindle was perpendicular to the carriage, but the entire transport assembly appears to not be fully aligned to the table base. The only way I can see to adjust it is with shims, or to face the whole table.

Here is the machine:

http://s1262.photobucket.com/user/Mo...slideshow/CNC2

If you look at the first photo, you see that the table seems to dip toward the lower left. It could also be that I just mounted the work poorly, among other things. The quick fix is to simply face the plastic block before the next run. Something I should have done first, but the block itself seemed pretty good.

"Do you have a link to the CNC machine you own?"

No. It seems to be hand built by the seller. There is "RT Technik" engraved on the front, but I found no web hits. Few of the components even have labels, but the seller says he got everything locally, and to contact him if I need any parts. Here in Germany there are maybe a dozen commercial manufacturers building machines like this, as well as many individuals making them in their garages and selling them on Ebay. I shopped for a year and this is what I chose. So far it seems like I did well. Much of the Mach3 controller software is still a mystery to me, but fortunately the seller walked me through the basics. The hardest part has been creating decent toolpaths using Bobcad26. I'm not sure that was a good decision, but I am getting the job done now, after like two months of despair.


"The hardest part has been creating decent toolpaths using Bobcad 26"

Right. That's because BobCADCAM is crapware. At best it is a cobbled together mess. BobCRAP only has one strong suit: They license the ModuleWorks surfacing toolpath engine and you can often buy BobCRAP very cheaply.

I would strongly suggest making contact with Al Depaolo for help with surfacing toolpath:

https://www.youtube.com/watch?v=6RFeoplaLMM

Al is easily the best guy they have. Tell Al I sent you. He knows how I feel about BobCRAP and he's still a member of my LinkedIn group even if he knows I frown on discussion of BobCRAP in my group because it's not an industry technology leader. One day BobCRAP's owner will finally wake up and realize that they will have to rewrite it from the ground up using a real geometry kernel like Parasolid, ACIS or CGM. Without that they will never have decent solid modeling.

If you are going to cut metals I would strongly suggest getting another machine to do it that's more rigid. Something like this perhaps?

https://www.youtube.com/watch?v=nev98v3PyXk

If you are going to cut metals I would strongly suggest getting another machine to do it that's more rigid. Something like this perhaps?

https://www.youtube.com/watch?v=nev98v3PyXk

That tool changer would be sweet. Otherwise I'm getting perfectly good results cutting brass now that I've worked out most of the kinks. And, the big XY plane means I can do lots of stuff I couldn't do on a normal knee mill.

Thanks for the tip on Al. I paid 1k for the Cad/Cam + BobArt. Not bad, but I paid another $400 for two hours of rather lame online training. Anyway, I'm now able to do everything I need, and some of my parts are rather complicated.

On Friday, February 27, 2015 at 12:21:51 AM UTC-8, robobass wrote:
If you are going to cut metals I would strongly suggest getting another machine to do it that's more rigid. Something like this perhaps?

https://www.youtube.com/watch?v=nev98v3PyXk

That tool changer would be sweet. Otherwise I'm getting perfectly good results cutting brass now that I've worked out most of the kinks. And, the big XY plane means I can do lots of stuff I couldn't do on a normal knee mill.

Thanks for the tip on Al. I paid 1k for the Cad/Cam + BobArt. Not bad, but I paid another $400 for two hours of rather lame online training. Anyway, I'm now able to do everything I need, and some of my parts are rather complicated.

Don't be so quick to discount knee mills with a sliding ram. They can be very versatile when you need to do large plates/parts.

Al's specialty is 3 axis surfacing toolpath. Many CADCAM systems use the ModuleWorks toolpath engine. Al knows the ModuleWorks toolpath engine very well as he's spent many years supporting it:

http://www.moduleworks.com/company/partners/

Don't be so quick to discount knee mills with a sliding ram. They can be very versatile when you need to do large plates/parts.

I did have a Boss3 for many years. What I have now fits my needs for my current situation very well. Here in Germany, a big knee mill is much more expensive than in North America, new or used. Also, all big industrial machinery here runs on 380-400v only, and I have to make do with a single 3.8KW 220v circuit for the whole shop. Riggers charge more too. A knee mill just isn't in the cards for me.

Al's specialty is 3 axis surfacing toolpath. Many CADCAM systems use the ModuleWorks toolpath engine. Al knows the ModuleWorks toolpath engine very well as he's spent many years supporting it:

I just watched a few of his videos. Very helpful!

On Saturday, February 28, 2015 at 2:28:45 AM UTC-8, robobass wrote:
Don't be so quick to discount knee mills with a sliding ram. They can be very versatile when you need to do large plates/parts.

I did have a Boss3 for many years. What I have now fits my needs for my current situation very well. Here in Germany, a big knee mill is much more expensive than in North America, new or used. Also, all big industrial machinery here runs on 380-400v only, and I have to make do with a single 3.8KW 220v circuit for the whole shop. Riggers charge more too. A knee mill just isn't in the cards for me.

Al's specialty is 3 axis surfacing toolpath. Many CADCAM systems use the ModuleWorks toolpath engine. Al knows the ModuleWorks toolpath engine very well as he's spent many years supporting it:

I just watched a few of his videos. Very helpful!


Glad to hear this!

It can takes a lot of effort to master surfacing toolpath because their parameters are often changed as developers improve them.

I create surfacing toolpath everyday and I still run into situations that I struggle with.

On Saturday, February 28, 2015 at 4:09:00 PM UTC+1, jon_banquer wrote:
On Saturday, February 28, 2015 at 2:28:45 AM UTC-8, robobass wrote:
Don't be so quick to discount knee mills with a sliding ram. They can be very versatile when you need to do large plates/parts.

I did have a Boss3 for many years. What I have now fits my needs for my current situation very well. Here in Germany, a big knee mill is much more expensive than in North America, new or used. Also, all big industrial machinery here runs on 380-400v only, and I have to make do with a single 3.8KW 220v circuit for the whole shop. Riggers charge more too. A knee mill just isn't in the cards for me.

Al's specialty is 3 axis surfacing toolpath. Many CADCAM systems use the ModuleWorks toolpath engine. Al knows the ModuleWorks toolpath engine very well as he's spent many years supporting it:

I just watched a few of his videos. Very helpful!


Glad to hear this!

It can takes a lot of effort to master surfacing toolpath because their parameters are often changed as developers improve them.

I create surfacing toolpath everyday and I still run into situations that I struggle with.

For me the surfacing itself isn't what's creating headaches, it's setting boundaries where I get hung up. And that goes for for some 2D profiling jobs as well!

On Saturday, February 28, 2015 at 12:21:24 PM UTC-8, robobass wrote:
On Saturday, February 28, 2015 at 4:09:00 PM UTC+1, jon_banquer wrote:
On Saturday, February 28, 2015 at 2:28:45 AM UTC-8, robobass wrote:
Don't be so quick to discount knee mills with a sliding ram. They can be very versatile when you need to do large plates/parts.

I did have a Boss3 for many years. What I have now fits my needs for my current situation very well. Here in Germany, a big knee mill is much more expensive than in North America, new or used. Also, all big industrial machinery here runs on 380-400v only, and I have to make do with a single 3.8KW 220v circuit for the whole shop. Riggers charge more too. A knee mill just isn't in the cards for me.

Al's specialty is 3 axis surfacing toolpath. Many CADCAM systems use the ModuleWorks toolpath engine. Al knows the ModuleWorks toolpath engine very well as he's spent many years supporting it:

I just watched a few of his videos. Very helpful!


Glad to hear this!

It can takes a lot of effort to master surfacing toolpath because their parameters are often changed as developers improve them.

I create surfacing toolpath everyday and I still run into situations that I struggle with.

For me the surfacing itself isn't what's creating headaches, it's setting boundaries where I get hung up. And that goes for for some 2D profiling jobs as well!


BobCRAP makes very poor use of the information a model contains so you often have to extract or create wireframe for your boundaries so you can cut what you want. Even in better CADCAM products, the need for creating boundaries is still there. As time goes on, and CADCAM products finally start to make better use of the information a model contains, the need for creating boundaries will be drastically reduced. In better CADCAM this is happening now and it's only going to get better:

Here are two videos that illustrate my point:

https://www.youtube.com/watch?v=FRDILRT3jx8

https://www.youtube.com/watch?v=jyyn6h_b-oY

Update. So after all of the tweaks, I think that going with a 6mm 4-flute carbide mill was the biggest single thing. I first rough a thru-slot with a 4mm mill to reduce the stress on the larger mill as well as allow chip clearance. Here you see just the roughing pass. 0.5mm cut depth per pass, and leaving 0.05mm for a full depth finishing pass. If you remember, I'm doing this with a gantry router. Works well enough!
http://i1262.photobucket.com/albums/...2/SlotFix1.jpg