Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

MULTIPLE CUTTER COMPS....


Recommended Posts

Hello all,
   I am using CONTOUR with MULTI PASSES and it shows CUTTER COMP every pass, where as I only want it shows on the "FINISH" and "SPRING PASSES" only not the "ROUGH PASSES"...  is there away that I can trick in the MasterCam2019 or editing the post?  If post then would you guys please guide me where to start?  I also attached the screenshot with annotations for details.

 

 

Thank you,
   S.Luong


============================ G-CODES====================

N31( .6250, 5/8 EM, CB, ROUGHER,)
(3FLTS 1.250LOC, 1.38STO)
G0 G17 G40 G49 G80 G90
G91 G28 Z0 M19
/G28 Y0.
T31 M6(ROUGH AND FINISH PROFILE, CUT#162)
G90 G54 S7500 M3
X-7.5266 Y.3448
G43(D31)H31 Z2. M8(DOC= Z-.515, .015 BREAK THROUGH)
Z.0625
G1 Z-.515 F100.
G41 D31 X-7.2153 Y.3176 ==================================> G41 D31, not needed...
G3 X-6.8767 Y.6016 R.3125
G2 X-6.8767 Y.6016 I6.8767 J-.6016
G3 X-7.1608 Y.9402 R.3125
G1 G40 X-7.4721 Y.9674
X-7.4917 Y.3417
G41 D31 X-7.1804 Y.3145 ==================================> G41 D31, not needed...
G3 X-6.8419 Y.5986 R.3125
G2 X-6.8419 Y.5986 I6.8419 J-.5986
G3 X-7.1259 Y.9371 R.3125
G1 G40 X-7.4373 Y.9644
X-7.4569 Y.3387
G41 D31 X-7.1455 Y.3115 ==================================> G41 D31, not needed...
G3 X-6.807 Y.5955 R.3125
G2 X-6.807 Y.5955 I6.807 J-.5955
G3 X-7.0911 Y.9341 R.3125
G1 G40 X-7.4024 Y.9613
X-7.422 Y.3356
G41 D31 X-7.1107 Y.3084 ==================================> G41 D31, not needed...
G3 X-6.7721 Y.5925 R.3125
G2 X-6.7721 Y.5925 I6.7721 J-.5925
G3 X-7.0562 Y.931 R.3125
G1 G40 X-7.3675 Y.9583
X-7.3871 Y.3326
G41 D31 X-7.0758 Y.3054 ==================================> G41 D31, not needed...
G3 X-6.7373 Y.5894 R.3125
G2 X-6.7373 Y.5894 I6.7373 J-.5894
G3 X-7.0213 Y.928 R.3125
G1 G40 X-7.3327 Y.9552
X-7.3523 Y.3295
X-7.1426 Y.3112 F5.
G41 D31 X-6.8312 Y.284 ==================================> This is good...... G41 D31, needed...
G3 X-6.4927 Y.568 R.3125
G2 X-6.4927 Y.568 I6.4927 J-.568
G3 X-6.7768 Y.9066 R.3125
G1 G40 X-7.0881 Y.9338
G0 Z2.
G91 G28 Z0. M9
/G28 Y0. M5
G0 G90 G54 X0.

1.png

0.png

Link to comment
Share on other sites

While I'm sure this can be done with the post, the easiest way would probably just to split it up into two different operations. Copy that toolpath below itself and make the first one roughing only with computer compensation and make the second toolpath the finish passes WITH wear compensation. That should easily do what you want it to do.

  • Like 2
Link to comment
Share on other sites

I would imagine so someone editing the file, does not have to change it on multiple lines or do a mass edit when using a different tool number. 

I wouldn't do it mainly because if you use a regrind the finish pass is now taking more than you anticipated. 

 

  • Like 1
Link to comment
Share on other sites
4 hours ago, Grimes said:

Im seriously questioning why it matters?

He means well, but will chase these things for weeks. I have asked this very question more than once about some of the things asked by him. Has good things he wants to do, but do ask the same thing how much of this is effort that could be focused else where. 

  • Like 4
Link to comment
Share on other sites
On 7/26/2018 at 12:06 PM, Frank Caudillo said:

While I'm sure this can be done with the post, the easiest way would probably just to split it up into two different operations. Copy that toolpath below itself and make the first one roughing only with computer compensation and make the second toolpath the finish passes WITH wear compensation. That should easily do what you want it to do.

Best suggestion and your done moving on to more important things. 

  • Like 1
Link to comment
Share on other sites

My HASP is at the office, but I think you could set a flag to suppress the output.  Set the flag by checking the total number of passes against the number of passes completed.

The total number of passes should be parameter 15560 + parameter 15380.  You can track the number of passes completed by incrementing a counter at null tool change if the op_id$ is the same.

On night this week I'll bring my HASP home and work up an example.

  • Thanks 1
Link to comment
Share on other sites

It can be done but as already said, best is to split in 2 ops. (or ask CNC a switch to calc rough passes with computer comp only...)

IMHO it can cause serious issues tweaking a post that way... you can count passes number set in Mastercam GUI but if CNC changes/improves routines in a future release (as it's been done in 2018 if I remember correctly) you probably will need to be careful (I ve already been bitten...) 

Another stuff to be aware: what if a user, one day, has great idea to post a toolpath with 'control' comp setting? It will make a crap part and a cutter broken...So don't forget to support that case in your post to output G41/G42.   

  • Thanks 1
Link to comment
Share on other sites
On 7/28/2018 at 9:54 AM, Grimes said:

Im seriously questioning why it matters?

Hi C^Millman,
   The reason I am doing it because I have to machine a "STEEL MAGNETIC BASE" which causing double cut when comp is presenting because CHIPS will come back and stick to the material.  Therefore, comping every time which leads tool to double cut material and parts become nonresistance as dimensional.

 

Thank you,
   S.Luong

Link to comment
Share on other sites
On 7/28/2018 at 12:42 PM, jlw™ said:

Are you simply trying to reduce NC file size or what?  I don't get it.

Hi JLW,
     The reason I am doing it because I have to machine a "STEEL MAGNETIC BASE" which causing double cut when comp is presenting because CHIPS will come back and stick to the material.  Therefore, comping every time which leads tool to double cut material and parts become nonresistance as dimensional.

 

Thank you,
   S.Luong

Link to comment
Share on other sites
On 7/26/2018 at 12:06 PM, Frank Caudillo said:

While I'm sure this can be done with the post, the easiest way would probably just to split it up into two different operations. Copy that toolpath below itself and make the first one roughing only with computer compensation and make the second toolpath the finish passes WITH wear compensation. That should easily do what you want it to do.

 

Hi Frank,
   I have tried that and it worked find.  On the other hand, when I leave .010 for roughing as steel magnetic, fine chips stick on and when i finish I have delete all upper comps to prevent in-consist dimensional changes.

Link to comment
Share on other sites
On 7/28/2018 at 2:24 PM, C^Millman said:

He means well, but will chase these things for weeks. I have asked this very question more than once about some of the things asked by him. Has good things he wants to do, but do ask the same thing how much of this is effort that could be focused else where. 

Hi JLW,
   Thank you for your reply, sometimes I have to deal with government material without given exact name.  I only guess and one of the material is very STICKY STEEL, having repeating COMPS causing tool to RE-CUT into more material.  I know I've been asking many "SILLY" questions but I guess I rather to having a bad name like that to get the knowledge that I don't have.


Thank you,
   S.Luong

Link to comment
Share on other sites
On 7/29/2018 at 6:37 AM, jeff.D said:

My HASP is at the office, but I think you could set a flag to suppress the output.  Set the flag by checking the total number of passes against the number of passes completed.

The total number of passes should be parameter 15560 + parameter 15380.  You can track the number of passes completed by incrementing a counter at null tool change if the op_id$ is the same.

On night this week I'll bring my HASP home and work up an example.

Hi Jeff,
   Thank you for your support, I truly appreciated.


S.Luong

Link to comment
Share on other sites
3 hours ago, PcRobotic said:

Hi C^Millman,
   The reason I am doing it because I have to machine a "STEEL MAGNETIC BASE" which causing double cut when comp is presenting because CHIPS will come back and stick to the material.  Therefore, comping every time which leads tool to double cut material and parts become nonresistance as dimensional.

 

Thank you,
   S.Luong

errrr, you lost me?

You've set mcam to finish with the one cut but rough with 4 passes of .035.

So how does the double cut happen? The machine is following true path with the .035 offset for each pass  - reducing to the finish cut - yes?

If you're getting chips stuck to the parts because of magnetism, this has nothing to do with comp?

Link to comment
Share on other sites

Hum when I have cut magnetic materials I have always had a clean out process for taking last cuts and trust me with enough air or high pressure coolant those chips will come out of the cut. Cheating the process creates problems and if the material requires a certain process like cleaning out the chips then that is what you do. Fugging a post to no get comp is not the answer and if the process were followed correctly for the material you are cutting then you could cut ti the same way day in and day out and never have a problem. In this case you don't have the correct process and what your doing is going to lead to more problems down the road than I see it solving, but I am the dumb person so I will just leave you to doing it the way you think it best.

Link to comment
Share on other sites
On ‎7‎/‎30‎/‎2018 at 2:52 AM, David Colin said:

It can be done but as already said, best is to split in 2 ops. (or ask CNC a switch to calc rough passes with computer comp only...)

IMHO it can cause serious issues tweaking a post that way... you can count passes number set in Mastercam GUI but if CNC changes/improves routines in a future release (as it's been done in 2018 if I remember correctly) you probably will need to be careful (I ve already been bitten...) 

Another stuff to be aware: what if a user, one day, has great idea to post a toolpath with 'control' comp setting? It will make a crap part and a cutter broken...So don't forget to support that case in your post to output G41/G42.   

Though I disagree that creating (and maintaining) two ops for this is the best solution, that's not why I'm responding.

You said you've been bitten by a change CNC made before, was it a change made to MP.dll?  Can you shoot me an email about this?  I'd like to help if I can.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...