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:

Trouble with Toolpath Transform

Sigurd

By Sigurd,
in Industrial Forum

 Share

Recommended Posts

Sigurd Enthusiast

Sigurd

Posted
Posted

Hello there. Today, I am cutting electrodes. There are four fixtures on the table, G54-G57. All I want to do is run the same program in the new WCS locations. I'm in the Toolpath Transform box and it seems like translating to a plane is the right way to go, but I'm not checking the boxes correctly. It will transform one time only, and both operations are G54. Can someone help with what I'm missing, please? Thanks.

Link to comment
Share on other sites
JParis Mentor

JParis

Posted
Posted
30 minutes ago, Rstewart said:

But two paths failed to end up in the code 🤔

In my experience, that is usually caused by paths that weren't either selected, they were ghosted or weren't in the transform..

I can't say that I have ever seen a post just leave out paths...

I utilize Transform HEAVILY!!!!

  • Like 1
Link to comment
Share on other sites
Sigurd Enthusiast

Sigurd

Posted
  • Author
Posted
On 8/11/2022 at 2:44 PM, AMCNitro said:

IMO it would be easier to copy and paste the TP and then just change the plane.  Create 4 toolpath groups and each group is a different WCS.

That's what I ended up doing on my second attempt. The first attempt was posting only G54, then copying, pasting and editing the WCS in the post. That's fine for only 7 ops, but what a pain. I think the guy before me copy and pasted at the control, but no one knows for sure.

Link to comment
Share on other sites
Leon82 Rising Star

Leon82

Posted
Posted
3 hours ago, Rstewart said:

Toolpath transform bit me today....

All seemed to post out correctly, But two paths failed to end up in the code 🤔  Didn't realize this until after the parts were off the machine.

This was just for g54 and g55 in two separate vises.  Could have been BAD.

Were they open pockets?

I had an issue with several jobs in 2020 that posted fine for 4 or 5 years in previous versions and then randomly would omit roughing passes. If I had actually followed the old set up sheet and used an insert mill instead of an accupro when we transferred it to our mam it would have exploded the cutter.

Link to comment
Share on other sites
JParis Mentor

JParis

Posted
Posted

This is, believe it or not, one of my easier "transform heavy" files...this is a part that runs

4 parts on each face

B0 - Prep OP - Mills Dovetail for mounting on fixture

B90 - OP1 Mills on B0, B90 & B180 faces

B180 - OP2 Mills on B180, B90 & B270 faces

B270 - OP3 - Mills on B270 face

As I work on the face say I am in OP 2....

I will work B90 - Top to Bottom

                  Rotate

                   B0 - Bottom to Top

                  Rotate

                  B180 - Top to Bottom

 

If the same tool then rotates to another OP and it left off at the bottom, that's where it will start keeping the same up/down motion at a tool change, it starts at the top and the process begins again.

My Individual part work offsets will ascend and descend based on my up or down direction....

Transform is incredibly powerful if you tap into it...like anything else, if you're looking for the quick thing and don't spend the time setting it up properly, you can and do fight it....

https://www.youtube.com/watch?v=nVQmIsDqD74

Apparently we can no longer embed YouTube videos???

That kind a bites

Link to comment
Share on other sites
Rstewart Apprentice

Rstewart

Posted
Posted
18 hours ago, JParis said:

In my experience, that is usually caused by paths that weren't either selected, they were ghosted or weren't in the transform..

I can't say that I have ever seen a post just leave out paths...

I utilize Transform HEAVILY!!!!

Man, all I know is I used the option to disable paths/ghost and create separate (or whatever it's called).  I've used it many times before, but I'm unsure of what could have happened??  Now I'm scared to use it.  It left off a 3d horizontal floor finish path and simple contour.  It may very well have been my fault, but I'm unsure of how or what...

Link to comment
Share on other sites
JParis Mentor

JParis

Posted
Posted
2 minutes ago, Rstewart said:

It may very well have been my fault, but I'm unsure of how or what...

Believe me, I get it...for me any way, when something out of the ordinary happens, I generally try to go back and diagnose what the heck I did....many times I figure it out. On those occasions where I can't, if it is repeatable, it's off the QC it goes.

Link to comment
Share on other sites
Sigurd Enthusiast

Sigurd

Posted
  • Author
Posted

I'm still having trouble translating to planes. I've got the planes defined, all with a new offset. Under the Translate tab, Between Planes is selected. I select the From plane (my G54 plane) and the To plane (my G55). If I green-check out of the box, and then go back in, the To plane has reverted to the G54 plane. What am I missing?

 

Link to comment
Share on other sites
JParis Mentor

JParis

Posted
Posted

OK, with what you're trying to do with this one, it's the simpliest of transform uses...

1. I deleted your planes...when you're posting for positions one on top of the other, it is unecessary..

2. Check out the settings that I used to get this...

I used the MPFAN psot and it posted as I expected

CwZvSE2.png

NX18PnO.png

 

 

O0000(MULTOFSTTEST)
(DATE=DD-MM-YY - 15-08-22 TIME=HH:MM - 09:44)
(MCAM FILE - C:\USERS\JOHNP\DESKTOP\MULTOFSTTEST (1).MCAM)
(NC FILE - C:\USERS\JOHNP\DESKTOP\MULTOFSTTEST.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T1 | 1 INCH FLAT ENDMILL | H1 )
G20
G0 G17 G40 G49 G80 G90
T1 M6
G0 G90 G54 X1. Y-3.5 A0. S534 M3
G43 H1 Z.25
Z.2
G1 Z0. F6.42
Y-2.5
G3 X0. Y-1.5 I-1. J0.
G1 X-1.
G2 X-1.5 Y-1. I0. J.5
G1 Y1.
G2 X-1. Y1.5 I.5 J0.
G1 X1.
G2 X1.5 Y1. I0. J-.5
G1 Y-1.
G2 X1. Y-1.5 I-.5 J0.
G1 X0.
G3 X-1. Y-2.5 I0. J-1.
G1 Y-3.5
Z.2
G0 Z.25
G55 X1. Y-3.5 Z.25 A0.
Z.2
G1 Z0. F6.42
Y-2.5
G3 X0. Y-1.5 I-1. J0.
G1 X-1.
G2 X-1.5 Y-1. I0. J.5
G1 Y1.
G2 X-1. Y1.5 I.5 J0.
G1 X1.
G2 X1.5 Y1. I0. J-.5
G1 Y-1.
G2 X1. Y-1.5 I-.5 J0.
G1 X0.
G3 X-1. Y-2.5 I0. J-1.
G1 Y-3.5
Z.2
G0 Z.25
G56 X1. Y-3.5 Z.25 A0.
Z.2
G1 Z0. F6.42
Y-2.5
G3 X0. Y-1.5 I-1. J0.
G1 X-1.
G2 X-1.5 Y-1. I0. J.5
G1 Y1.
G2 X-1. Y1.5 I.5 J0.
G1 X1.
G2 X1.5 Y1. I0. J-.5
G1 Y-1.
G2 X1. Y-1.5 I-.5 J0.
G1 X0.
G3 X-1. Y-2.5 I0. J-1.
G1 Y-3.5
Z.2
G0 Z.25
G57 X1. Y-3.5 Z.25 A0.
Z.2
G1 Z0. F6.42
Y-2.5
G3 X0. Y-1.5 I-1. J0.
G1 X-1.
G2 X-1.5 Y-1. I0. J.5
G1 Y1.
G2 X-1. Y1.5 I.5 J0.
G1 X1.
G2 X1.5 Y1. I0. J-.5
G1 Y-1.
G2 X1. Y-1.5 I-.5 J0.
G1 X0.
G3 X-1. Y-2.5 I0. J-1.
G1 Y-3.5
Z.2
G0 Z.25
M5
G91 G28 Z0.
G28 X0. Y0. A0.
M30

JP_multofsttest.mcam

  • Thanks 1
Link to comment
Share on other sites
JParis Mentor

JParis

Posted
Posted
3 minutes ago, Sigurd said:

You must have seen that post before I edited it! I fixed that one myself. So that's what "Disable posting on source operations" means; it ghosts them, and then you post the Transform op only.

Yes, it makes the op/ops part of the transform....you do NOT have to use it that way, you can leave it unghosted and change your transform value by 1 but I just find in cleaerer and cleaner to add it

  • Thanks 1
Link to comment
Share on other sites
Rstewart Apprentice

Rstewart

Posted
Posted
On 8/13/2022 at 9:02 AM, JParis said:

Believe me, I get it...for me any way, when something out of the ordinary happens, I generally try to go back and diagnose what the heck I did....many times I figure it out. On those occasions where I can't, if it is repeatable, it's off the QC it goes.

Well, I have one for QC....

Two parts, g54 g55.  I hear the finishing 3/4 endmill making more noise than it should be.

I go through the code and found the issue. On one operation (simple contour) it runs that path Twice on the G55 and never even calls out G54.  I have checked everything I know twice.  

 

Does anyone here wanna check it out??

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...