Jump to content

Welcome to eMastercam.com
Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.
Login to Account Create an Account
Photo

haas V5 cutter comp / 3d contour

- - - - -

  • Please log in to reply
15 replies to this topic

#1
ChrisH

ChrisH

    Member

  • Members
  • PipPip
  • 74 posts
I’m Programming for a hass and trying to cut a 3d contour with G41 cutter comp with Mastercam 9.1 and the mill gets a comp error. This is a exp.

code:


N16218T3M6(T3 - 2D-CONTOUR - 25.4 DIA)
N16220H3Z225.6508
N16222M3S450
N16224G0X-4.2324Y57.956
N16226M8
N16228Z128.6508
N16230G1Z85.6671F400.
N16232G41X14.8166Y58.1511F150.
N16234X21.1267Y58.2157
N16236G2X21.2611Y58.2163I.1351J-13.1994
N16238G1X45.3105Y58.2176Z84.948
N16240X57.3353Y58.2182Z84.5951
N16242X69.3477Y58.2189Z84.2427
N16244X69.3601Z84.2423
N16246X72.5303Y58.219Z84.1501
N16248X75.3726Y58.2192Z84.0686
N16250X78.1691Y58.2194Z83.9933

I can't see anything wrong with it.
graemlins/headscratch.gif

#2
JParis

JParis

    Advanced Member

  • Members
  • PipPipPip
  • 24,299 posts
Have you tried the path without the G41?

#3
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
Just looking at it real quick, I don't see a "D" in the program.

HTH

#4
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
%
O777 (TEST )
(TEST )
(DATE - 27-08-05 TIME - 10:08 )
( 3/8 FLAT ENDMILL TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - .375 )
G20
G0 G17 G40 G49 G64 G80 G98 G90
G0 G90 G54 X0. Y1.3988 S4074 M3
G43 H2 Z1.
M8
Z.9863
G1 G41 D2 X-.2438 F39.1
G3 X0. Y1.155 I.2438 J0.
G1 X1.7419
G2 X1.7569 Y1.14 I0. J-.015
G1 Y.946
G2 X1.7546 Y.938 I-.015 J0.
X0. Y-.0266 I-1.7546 J1.1134
X-1.7546 Y.938 I0. J2.078
X-1.7569 Y.946 I.0127 J.008
G1 Y1.14
G2 X-1.7419 Y1.155 I.015 J0.
G1 X0.
G3 X.2438 Y1.3988 I0. J.2438
G1 G40 X0.
G0 Z1.
M5
G49 Z1.
G91 G28 Z0. M9
M30
%

Here is a sasmple for a haas I get using cutter comp. Notice The D for your cutter dia on the G41 line.

graemlins/cheers.gif

#5
Crazy^Millman

Crazy^Millman

    Regular Guy

  • Members
  • PipPipPip
  • 12,032 posts
  • Location:Murrieta Ca
If the D was called before then it would default to the last one run in the program if you have not called one for that tool which it looks like you have not. So if you by chance have D3 for T2 if you post is not set to force out a D at toolchanges then it would not give you one here and would give you an alram because it is too big or too small which probaly saved your but.

HTH

#6
Kannon

Kannon

    Advanced Member

  • Members
  • PipPipPip
  • 4,734 posts
Good call Midwest!
graemlins/cheers.gif

#7
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
too big

+1

That could be it also

#8
ChrisH

ChrisH

    Member

  • Members
  • PipPip
  • 74 posts

code:


N650M06T03H03
N652G00X-258.075Y142.61M08
N654S450M03
N656G43Z193.387
N658Z96.387
N660G01Z55.361F400.
N662G41D03X-239.025Y142.684F150.
N664X-232.569Y142.709
N666X-229.34Y142.72Z55.355
N668X-227.724Y142.725Z55.354
N670X-226.108Y142.73Z55.344
N672X-224.493Y142.734Z55.353

I had a G41D03 in the program I took it out trying different things and forgot to put d03 back before I posted it on the forum. It still will not run with a D03 and .236mm in the mill comp.
I didn't know if you can keep cutter comp on with an X Y and Z move.
I'm going to take the haas book home today see if I can find some more on what the comp limits are. For now I’ll just change the program to match the regrind cutter. wink.gif

#9
Cadcam From Cad/Cam Consulting

Cadcam From Cad/Cam Consulting

    Advanced Member

  • Members
  • PipPipPip
  • 8,761 posts
Try post it with "Plung after first Move" in the lead in lead out and see how that goes.

#10
Jean-Simon

Jean-Simon

    Member

  • Members
  • PipPip
  • 257 posts
Ask Haas if it's a parameter or an option because works well here anywhere my D is.

Simon

#11
ChrisH

ChrisH

    Member

  • Members
  • PipPip
  • 74 posts
ok I found the problem I can't find a fix. I changed my linearization tolerance up to .1mm and it still puts in this small move (last line on the code Z moves) exp.

code:


 
Metric
N001(202706_FD-E_D826_20JUL05_CRH.mc9)
N002(FIX826OP1 POSTED FOR Haas)
O0000
N003G90G80G40G00G53
N004M06T03H03
N005G00X-43.586Y116.851M08
N006S450M03
N007G43Z171.212
N008Z74.212
N009G01Z55.685F400.
N010G41D03X-24.547Y116.199F150.
N011X-10.997Y115.735Z53.289
N012X0.774Y115.343Z51.229
N013X18.995Y114.728Z48.106
N014X19.004Z48.104
N015X19.01Z48.103

Is this something that I can change in the post?
confused.gif

#12
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
If you change your cutter dia in the machine to Zero, will it run the program??

If it does try using the wear option for cutter comp.

HTH

#13
ChrisH

ChrisH

    Member

  • Members
  • PipPip
  • 74 posts
I tryed comp at 0 and It runs if I have any amount in wear it give a cutter comp error.
The moves that is errors on are only .001mm moves. Is there a place I can limit the amount a small moves in mastercam?

#14
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
You could try using the filter option. Small moves and cutter comp don't work well.

Putting your file on the FTP site might help solve your problem. There are lots of quality people here that can help.

#15
ChrisH

ChrisH

    Member

  • Members
  • PipPip
  • 74 posts
My works internet blocks the ftp site. I'm going to take it home and upload it from there. Im leaving to go camping after work today so I can't do it till Monday.
Thanks Midwest have a good weekend.

#16
Midwest

Midwest

    Advanced Member

  • Members
  • PipPipPip
  • 5,104 posts
If you want you can e-mail the file to me and I can put it up for everyone to see. Zip if you can.

graemlins/cheers.gif