[Donkey Hotey]

I'm having the same problem. I created a very simple, single line contour path. I did the translate operation, told it to start with '0' as the first offset. I tried -1 as well as +1 as the increment amount. It still posts G55 first, then G54.
(MCX, Level 3, SP2)

[pp-TG]

CadCam,

I will try and get it off the work computer if i can get the ok to do so and post it. It also looks to me like it is not what i am doing but what my post is doing with it, i think it is the post i am using i tried the same configurations with a generic fanuc post and got a different out come so i believe it is the post. Is this possible?

Thanks,

[cadcam]

pp-tg, I understand that is why I want the post to to see if this an issue I can fix to.

[pp-TG]

CadCam,

Hay thanks for all your help i did get everything fixed and it is working great it turns out it was a little bit of post and a little bit of my settings mostly post.

Thanks again for all your help and time...Would have never got it otherwise.

[Donkey Hotey]

OK, now it's my turn.

I got the offsets to work correctly (Start offset: 1, Increment: 1).

Now my next question:
If I were to do this type of operation, I'd imagine that it might be for multiple parts in similar vises.

How do I change the sort order of the operations so it does the first operation on both vises at once (G54, G55)? Right now, it does all of the operations at G54, then moves over to G55 and repeats the whole path over again. That doubles the number of tool changes and adds to the cycle time. If it's already got T1 in the spindle, I want it to go over and machine the second part while it's at it. :withstupi

[Geof]

OK, now it's my turn.
....
If it's already got T1 in the spindle, I want it to go over and machine the second part while it's at it. :withstupi

You go to this thread:

http://www.cnczone.com/forums/showthread.php?t=51582

and look at the program.

Basically all your tools and their operations are in individual subroutines; you set the work zero and go to the tool subroutine and just keep repeating this through all the work zeroes. Then cycle through for the next tool. You can call different subroutines for the same tool to do different operations and offset the Z in the work zero (or with a G52 command).

[Donkey Hotey]

Thanks Geof.

Actually, I know how to do it manually but I'm trying to find out if Mastercam can output it that way.

I will read-up on the G52 stuff though. I've been curious about that and it may have other applications for me (maybe even some 5th axis stuff).

[Donkey Hotey]

Holy cow, what a complicated mess (trying to figure this out). I've been at this for hours and had authored a long post, documenting what I tried, ready to ask for help again, then I stumbled onto the solution. :withstupi

The premise:
Three vises on the mill, three sequential work offsets (one for each) and three identical parts to be run at the same time. The toolpath should do the same operation on each vise, moving from one to the next, while it has each tool loaded.

The solution:

• Type is Translate
• Method is Tool Plane (a grid of locations on a common tooling plate or tombstone would be Coordinate). On my Haas, I'll have identical workstops and parallels on each vise and each will have its own work offset (G54, G55, G56).
• Group NCI Output by Operation Type: It sorts how the output is grouped. Operation Type does each operation one time, at each vise, before moving to the next operation. Operation Order goes through the whole part, once at the first vise, then does everything over again on the second and so on. This is wasteful because it goes through all the tool-changes three times.
• The most important part I was missing was the upper right of the dialog: Copy Source Operations and Disable Posting in Selected Source Operations. What this does is disable posting the individual toolpath operations (if you don't pick this, you get an extra pass over all of the parts in the first work offset). They exist solely to supply input to the Translate operation. When they're disabled, the Translate operation goes through the disabled statements over and over, generating the tool moves for each tool.
• The Work offset numbering has to be turned on, has to start with zero (0) and increment by 1.

What a mess to try to figure out from the help. Well, at least it can do it. I know how to do it now. Now that I've posted this, I'll be able to look it up again when I finally need to use this and I've forgotten it.

[rickyt]

Yeah, I wish they would come up with a better way to do this. To many steps and easy to miss something and have to go back and try again. It really sucks if you have a horizontal mill and trying to machine complete parts around the tombstone (b0 is op one, b90 is op two and so on).

[Donkey Hotey]

How do you handle the tombstone faces? Do you assign a new work offset to each face or do you index the tombstone from the program?

[cadcam]

Greg Sorry I did not have more time lately to answer your question. I teach this every year as I always get the same question. I was thinking I was going to have time to create a quick video and did not.
Sorry as I feel I let you struggle.

As for Horz programming it matters if you program to center of rotation or to one part.
If you are doing a family of the same part you would use the option of Transform but with the rotation instead of transfer.
When programming Horz if the post is set for Horz you program by Named planes for different rotations.
I do allot of Horz program with multi pallets and multi setups on the tomb stones. so one program hits let say 4 diffrent stations and then is done.

there are a few different ways to go after Horz programming. I find it makes a difference on the part how many parts and options for holding and what the shop I am programming is used to working.
The one am at now they want a sep G10 offset for every part and rotation. the last one I programed being valve body had 2 stations on one pallet and another fixture on another pallat call up. this had 17 offset G10s.

[Donkey Hotey]

Greg Sorry I did not have more time lately to answer your question.

Absolutely no sweat, Jay--Really. You've been far more help to me than I can tell you. CNC Software should be paying you to provide the support you do here.

The hours of fumbling around got me through all of the options in the dialog box. That was actually more valuable than being shown the answer. I also learned a bunch of other things that I didn't know. It was a productive day.

[cadcam]

How do you handle the tombstone faces? Do you assign a new work offset to each face or do you index the tombstone from the program?

I do both matters on what the customer wants. or a different G54.1 series offsets for each part.

[facegarden]

Holy cow, what a complicated mess (trying to figure this out). I've been at this for hours and had authored a long post, documenting what I tried, ready to ask for help again, then I stumbled onto the solution. :withstupi

The premise:
Three vises on the mill, three sequential work offsets (one for each) and three identical parts to be run at the same time. The toolpath should do the same operation on each vise, moving from one to the next, while it has each tool loaded.

The solution:
...

• Type is Translate
• Method is Tool Plane (a grid of locations on a common tooling plate or tombstone would be Coordinate). On my Haas, I'll have identical workstops and parallels on each vise and each will have its own work offset (G54, G55, G56).
• Group NCI Output by Operation Type: It sorts how the output is grouped. Operation Type does each operation one time, at each vise, before moving to the next operation. Operation Order goes through the whole part, once at the first vise, then does everything over again on the second and so on. This is wasteful because it goes through all the tool-changes three times.
• The most important part I was missing was the upper right of the dialog: Copy Source Operations and Disable Posting in Selected Source Operations. What this does is disable posting the individual toolpath operations (if you don't pick this, you get an extra pass over all of the parts in the first work offset). They exist solely to supply input to the Translate operation. When they're disabled, the Translate operation goes through the disabled statements over and over, generating the tool moves for each tool.
• The Work offset numbering has to be turned on, has to start with zero (0) and increment by 1.

What a mess to try to figure out from the help. Well, at least it can do it. I know how to do it now. Now that I've posted this, I'll be able to look it up again when I finally need to use this and I've forgotten it.

Just stumbling onto this myself...
So the Work offset number starts at zero and increments by 1... but how do you tell it to do it 3 times? I can't get this to work because I don't know how to tell it how many work coordinate systems to use! :-/
Thanks,
-Taylor

[Donkey Hotey]

You don't tell it how many offsets to use. It does that automatically. You tell it how many copies to make in the Translate tab, by inputting the number of "Steps" you want.

[facegarden]

Hmm... Well I have my "Type and Methods" tab set up identically to you, and my "Translate" tab is set up to "Rectangular" with arbitrary x and y spacing, with 4 X steps and 1 Y step, no "Pattern origin shift". and no "Views" selected.

When i rebuild the operation i get 4 copies of the toolpath shown in mastercam all spaced evenly 2" apart like my X spacing shows. When i post, there are no G54, G55, G56 commands, it just repeats the op 2 inches over, then 2 more inches over, then 2 more inches over. What gives? We should be seeing a G54,55,56, right?

Thanks for your help, I can post screenshots or files if necessary, but I would love to get this figured out!
-Taylor

[Donkey Hotey]

Are all of the settings the same as in this dialog snapshot? Pay particular attention to the Work Offset Numbering on the lower right and the copy options on the upper right. I beat my head against the wall trying to get this right so don't feel bad.



What kind of machine are you trying to run on and what post are you using? It's possible that it's a problem with the post not supporting additional work offsets.

[facegarden]

Yeah, all the settings are the same. I'm using the "Generic HAAS 3 axis" post for a haas VF-2.

Playing a bit more, it seems that even if I have two operations using different WCS's, it doesn't seem to post. Is there something I need to modify in the post to get it to use multiple WCS's?
Thanks,
-Taylor

[riverracer]

try the setting "between points" on the translate page.
then "steps" = the extra positions + the original part.
eg: example attached should give you 3 positions @ G54, G55, G56 in your post.
(well it does on/with my HAAS post)

i have been testing examples and following this post for a while as well.

thanks all

[Donkey Hotey]

Yeah, it looks like you're going to need to post the file or send it directly to me. I can't look at it until tonight. PM me if you can't post it for whatever reason and need my email address.