Hello Guest it is October 17, 2019, 02:02:34 AM

Author Topic: Cutter Compensation  (Read 35777 times)

0 Members and 1 Guest are viewing this topic.

Offline Sage

*
  •  365 365
    • View Profile
Re: Cutter Compensation
« Reply #30 on: October 23, 2008, 09:00:03 PM »
First off thanks Graham for another version that works. I'll use the technique when the necessity arises.

BUT:

Lets all get on the same page.

I know I tend to type too much and nobody wants to read it all but:

Back at the beginning I think I explained that the path you see is already offset for a 1/8 cutter. I used LazyCam offset feature for a 1/8 cutter on the original DXF file to get the path you see. Therefore if you cut the profile as it is with a 1/8 cutter following the toopath shown the resulting part will be in the middle (.0625") smaller in all directions.

When I ran it, it was too slow and I was having trouble with chips binding up so decided I should use a 1/8 hogging mill to do a rough pass around the part and leave a bit for a finish cut.

 Rather than go back to nasty old LazyCam and generate another set of code for a bigger offset path to stay out a few thou to rough and then have two sets of code I decided to try the tool compensation feature.

This is exactly what it's intended for (as I understand it)

That's why I'm trying to generate another path only .020 (or even less) around the part. I chose .020 because you don't have to zoom the toopath screen so much to see it and to identify the "problem" which appears. (I'll change it to about 5thou later)

I wanted to use a subroutine so I could call the same code to do both paths, with and without the compensation.
I like to strive toward compact and elegant code if possible rather than having several hundred lines to do the same thing.

 I guess I / we have to start this discussion all over.

So  - how do you create a new path for a 1/8 cutter using cutter compensation so as to leave say 5thou all around the existing profile ?

Sorry for the confusion

Sage

Offline Graham Waterworth

*
  • *
  •  1,889 1,889
  • Yorkshire Dales, England
    • View Profile
Re: Cutter Compensation
« Reply #31 on: October 24, 2008, 06:19:49 AM »
The code I posted is commanded on the cutter centre line NOT an offset path, so to run the same cutter round to take a small amount more off you would change the cutter dia in the offset table from .125 to .105 and this would then remove another .02" from the part.

Graham
Without engineers the world stops

Offline Sage

*
  •  365 365
    • View Profile
Re: Cutter Compensation
« Reply #32 on: October 24, 2008, 08:53:13 AM »
Graham:
 Thanks again for the code. I have learned something from it as I now see how the cutter compensation takes effect on the first move.

Unfortunately your code shows the same problem as mine. You probably didn't notice it or there is something messed up with my default settings causing it.

First off there is some very annoying red line extending up a long way from the part that makes it necessary to zoom the image instead of it auto sizing to fit the preview screen. Not sure what causes that. But we can ignore that for now unless you know how to fix it. It will help make troubleshooting less annoying if you can.

To see the problem I'm talking about:
Load your code and then set cutter #1 to .020 (small I know but it should be valid if I want to take just a small extra cut).

Zoom in VERY VERY close on the bottom left corner and run the code.
You will see the cutter come in from the right and stop too soon. It rises up along the vertical line ON THE LINE and slowly tapers out to the left as it rises (as if cutter compensation turned off and back on again).
 This is not a display anomaly as you can also see it in the DRO's as well. The X DRO should be stationary as it rises along the Y axis because it is a square corner. The DRO is constantly counting negative all the way up the left side. It eventually reaches the correct position when it gets to the top .

If you don't see this let me know. I might have to check my default settings.

Sage

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Cutter Compensation
« Reply #33 on: October 24, 2008, 09:08:49 AM »

To see the problem I'm talking about:
Load your code and then set cutter #1 to .020 (small I know but it should be valid if I want to take just a small extra cut).

Zoom in VERY VERY close on the bottom left corner and run the code.
You will see the cutter come in from the right and stop too soon. It rises up along the vertical line ON THE LINE and slowly tapers out to the left as it rises (as if cutter compensation turned off and back on again).
 This is not a display anomaly as you can also see it in the DRO's as well. The X DRO should be stationary as it rises along the Y axis because it is a square corner. The DRO is constantly counting negative all the way up the left side. It eventually reaches the correct position when it gets to the top .

If you don't see this let me know. I might have to check my default settings.

Sage


As I said yesterday, it appears to be a bug related to the small tool diameter, because it appears to work correctly with a 1/8" tool.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Cutter Compensation
« Reply #34 on: October 24, 2008, 09:12:32 AM »

That's why I'm trying to generate another path only .020 (or even less) around the part. I chose .020 because you don't have to zoom the toopath screen so much to see it and to identify the "problem" which appears. (I'll change it to about 5thou later)


When using comp, you code for the actual part size, with no offsets. If you want to do a rough pass with a 1/8" tool, set up a too in mach3 with .165 diameter, but actually use a .125 tool. This will leave .02 around your part. Then go back and cut your finishing pass, telling mach the tool is .125, and it will cut to size. Same g-code, just use a different tool in the tool table, but they can actually be the same tool.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline Sage

*
  •  365 365
    • View Profile
Re: Cutter Compensation
« Reply #35 on: October 24, 2008, 10:16:03 AM »
Ok - got it.
 The light went on with your explaination of how this is all supposed to be used.
I have the concept now and it makes more sense. Sorry it took ten pages of back and forth for it to sink into my thick skull. I guess I was devising a concept of how to do the job with the tools at hand, saw the offset feature of LazyCam and figured that's how I'd do it. Your process, now that you explain it, is much more sensible. Hopefully others will learn from this. According to what I've read, tool compensation is one of those things people give up on understanding.

Sorry I hijacked the thread but I did set out to quickly point out another example of the problem the thread was started for (honest).


Thanks to both of you.


SO now that we have confirmed that there is a problem (even though it may never be seen because such a small tool is unlikely)...

Is there anyone keeping a master list of all of these issues discovered / suspected / eluded to, so they can be investigated and corrected or are they all scattered amongst the thousands of posts on this site never to be found again?

Mach is a very excellent program. I hope to see it get closer to perfect.

Sage

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Cutter Compensation
« Reply #36 on: October 24, 2008, 11:24:23 AM »
Hopefully Brian has a list, that he will be using to fix the issues shortly. :)

Quote
The light went on with your explanation of how this is all supposed to be used.

How it's supposed to be used is very subjective. As long as it works for you (once you understand how it works), you can use it any way you want. :)
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline Graham Waterworth

*
  • *
  •  1,889 1,889
  • Yorkshire Dales, England
    • View Profile
Re: Cutter Compensation
« Reply #37 on: October 24, 2008, 12:59:55 PM »
Hi guys,

even setting the tool dia to .005" on my system the path is perfect, I have Mach set to G61 (exact stop mode) if I set it to G64 (CV mode) I get rounded and miss formed profiles.

O0001 (SAGE BUSHING)

G20 G40 G00 G80 G17
G61

N1 (FLAT -  1-8 IN DIA)
T1 M6
G00 G90 G43 X0 Y0.569
Z0.1
S4500 M3
Z0.05
G01 Z0 F2.
M98 P0002 L19
G00 Z1.
G91 G28 Y0 Z0
M30
 
O0002 (CONTOUR SUB)
G91
G01 Z-.02 F2.
G90
G41 D1 X-0.141 F8.
Y0.491
G03 X0. Y0.35 R0.141
G01 X0.217
G02 X0.392 Y0.175 R0.175
X0.217 Y0. R0.175
G01 X0.
Y0.35
G03 X0.141 Y0.491 R0.141
G01 G40 Y0.569
X0
M99

Graham
Without engineers the world stops

Offline Sage

*
  •  365 365
    • View Profile
Re: Cutter Compensation
« Reply #38 on: October 24, 2008, 02:23:03 PM »
Definately a problem here.
I tried the G61 at the start of your program and it did not help here.
I still see X changing as it goes up the left side. Cutter set for .005.
He attached screen shot shows the bottom left corner how it comes across bottom with compensation and then goes up left side without it but slowly tapers back out to left as it rises.

I've atached my xml file maybe you can see something I'm missing. It's off my test laptop. I haven't tried your code on my actual mill.

(the attachments were an after thought look carefully hey are both there. One is above the picture.)

Maybe Gerry would be so kind as to try it.

You say Brian probably has a list. I was wondering how Brian is finding out about the issues. Are you guys making him aware?

Sage




« Last Edit: October 24, 2008, 02:36:33 PM by Sage »
Re: Cutter Compensation
« Reply #39 on: October 24, 2008, 02:37:18 PM »
Been following intently.
Great topic.
Just copied Grahams last code and get the same as Sage.
Strange.
RC