HMC programming training?

[Sticky]

If I am understanding Joe's problem correctly:

 

In this first picture the yellow grid is the start of my transform op (B90), so that my last B axis index is B0.

 

 

My next operation starts on B0, and thus the spindle attempts to become one with the tombstone

 

[Colin Gilchrist]

My post IS set for full retract on index for the reasons you mentioned! The issue is that I was on the LEFT side of the tombstone, MC ignored the "clearance" value and almost sent my spindle into the tombstone/parts sitting on B0. Luckily I was watching the code like a hawk, and I saw it coming before it happened. What makes this particularly dangerous is that I had a few other tools going to the same plane, and because they had more then two entities, they used the "clearance" value, just like they SHOULD. If I had been the slightest bit complacent in thinking "MC/post is working as it should as shown by the previous tools" I'd be out over 50k right now.

 

 

 

Glad to know I'm not the only one... Yikes.

 

 

 

I sent it to In House. Is there someone else I can send it to? In house doesn't give me bug #'s.

 

 

Joe, I can replicate your problem with my MPMASTER post.

 

It really sounds like this isn't the fault of the post. If the toolpath doesn't output the move, then there is nothing for the post to output. So it sounds like a toolpath bug. I've seen this with Drill Toolpaths, that only drill a single point. You should report this to 'QC(at)Mastercam.com'. I would recommend requesting a bug number. Keep in mind that when this does get fixed, it will be in X8 or later.

 

You can get around that a couple ways. You could read the clearance value from the Operation Parameters, and add some logic to always output the clearance value from the operation between operations. We could also setup a Miscellaneous Real Number in the operations and read the value from there.

 

Another option I've seen is to setup a User Defined Reference position, like "G30" or "G30 P1-P4", and just force the post to output that code between operations so that the machine always goes to a safe position before indexing.

 

Working with Transform Operations can be tough. I think James Meyette made a detailed post recently on how he setup the Transform custom parameters to handle the output for work offsets. I'm a fan of doing this as well, so that you have explicit control over your output.

[Sticky]

Ok I'll send a file to QC and see what they say.

 

I'm not following what you are referring to by "Operation Parameters"? I assume you aren't talking about right clicking on the tool path, edit common params?

[Colin Gilchrist]

All of the data that you enter into the Mastercam Toolpath Dialog boxes can be accessed by the Post Processor using functions available to the post writer.

 

In the post block 'pparameter$', logic can be added to capture the numeric values entered in the data entry fields in the operation dialog. These values can be held in user-defined variables, and used by the post writer for any purpose they wish. So it is technically possible to modify the post processor to read the values you entered into the dialog, and then output whatever values you wish.

 

I mention this because it would be possible to overcome the bug with not outputting the Clearance value before the rotation occurs.

 

It would be better in the long run if the bug with not outputting the Clearance value is fixed, and the value is output to the NCI file.

 

There are options in every toolpath dialog box that allow you to pass data to the post processor. There are Integer values called "Miscellaneous Integers" and numeric values called "Miscellaneous Real Numbers" where the user can enter data, and have that data be loaded into pre-defined variables, making them available to the post writer.

 

Using a combination of math and logic, there are almost unlimited possibilities when it comes to writing posts for Mastercam, and what you can do for custom output.

[MIL-TFP-41]

I still am curious about this potential issue. I have tried to duplicate tho I cannot manage....Maybe I am doing things different?

[Joe788]

I still am curious about this potential issue. I have tried to duplicate tho I cannot manage....Maybe I am doing things different?

 

Find one of your existing files that has four identical parts, one on each face of a four sided tombstone.

 

Create a toolpath that cuts on the right side of the part (Tombstone will Index to B90).

 

Use Toolpath>Transform>Rotate that toolpath so it runs on the right side of the other three parts.

 

Create a toolpath that works on the front of the part with the same tool as the previous toolpath. (Tombstone at B0).

 

Transform>Rotate that so it works on the front of the other four parts.

 

When you post - it will move from the 4th instance of the right side program, to the first instance of the front program, without sending it home (since there's no B index, so it won't tell it to go home). KABOOM.

[Sticky]

JMC, are you talking about Joe's problem? I should mention that when I do what Joe is talking about it at least still uses the clearance value in the Linking parameters. So not sure if its a bug as much as watch out type of problem.

 

The problem I am having on the other hand is really simple to test. make ONE drill tool path on a wcs like this:

 

 

Set Linking parameters like this:

 

 

Now make another wcs, and use the same tool and parameters to do the same thing on the new wcs:

 

 

And for me I get code like this:

 

 

^ Between N45 and N50 there SHOULD be a Z2.0 called.

 

 

If you make two drill points with the same tool paths and planes you get the correct retract like this:

 

[Sticky]

 

When you post - it will move from the 4th instance of the right side program, to the first instance of the front program, without sending it home (since there's no B index, so it won't tell it to go home). KABOOM.

 

In the sample I made trying to mimic your problem it still uses the clearance values, does it use them on your end?

[CJep]

I've been using the home /reference points to retract and approach in the Z axis,..

I don't typically activate the clearance in the linking parameters,...

For multiple offsets on the same face I group the transforms by tool number.

 

I use the MpMaster post

[MIL-TFP-41]

ahhhh...I think I get it. Like in this example?

CRASH TEST.MCX-7

[GoetzInd]

Yep just checked our mpmaster based posts. Would go right through the part. Thanks for the heads up.

 

Mike

[Sticky]

JMC and Goetz, are your programs using or ignoring the "clearance" value?

[Colin Gilchrist]

Hi Dave,

 

I created an example of what I meant by "operation parameters". Here is a test file that has a single drill operation on G57, and then has an operation with 2 drill points on G55. I added some code that forces out the clearance value, when you have a drill operation, that has a single point of geometry, and you've told the operation you want "clearance" on, but only at the "start and end" of the operation. (It would be easy to modify the logic to only check to see if the Clearance is on, regardless of the 'start/end only' value).

 

The PDF file explains the post changes I made to be able to force out the clearance value.

 

Hope that helps,

 

Colin

SINGLE DRILL POINT CLEARANCE FIX.Z2G

Post fix for forcing Clearance Value.pdf

[Newbeeee™]

Nice work Colin and excellent pdf.

[Colin Gilchrist]

Thanks Newbeeee. I hope it helps...

[Sticky]

Wow Colin, you are the man! You really did a nice job on that .pdf

 

I'll try adding it into my post tomorrow.

[?Mark]

Colin is one of the most patient, helpful, knowledgeable and eloquent guys on this board.

<cheers>

[Colin Gilchrist]

Thanks so much for the kind words guys. I just really enjoy helping other Mastercam users. I think Dave made a comment in another thread about how you need to be a software engineer to be able to modify the posts in Mastercam to get the output you need. I think he is absolutely correct about that. Machines and their control units have been getting more advanced for years, and to some extent the software has also become more complex in order to harness the new power available in the machines.

 

Mastercam is incredibly powerful, but you've got to have a good post processor to take advantage of that power. So it either falls to an outside vendor to understand your processes and needs, and create a post for you, or someone in your company has to do the job. That was the reason I created my original "Basic Post Processing" classes, because there aren't many resources for the average programmer to learn how to edit posts, and it is such an essential skill for so many shops.

[Sticky]

Well I think I know who will be giving me some training in the near future

[DUM1]

DODGED THE CRASH PROBLEM A FEW TIMES BY USING THE APPRAOCH POINTS IN THE HOME REF / POINTS , GOTTA SEE IT COMING THOUGH

[guitar]

G10 output for WCS's based off COR

Extended workoffsets

A method of being able to transform rotate a transform translate op with extended offsets

Productivity plus integration

 

Those are just some of the things that someone who would want to take this course is going to need help having integrated into their post. Sounds like you won't have any problem doing that, but I thought it was worth mentioning because other people will have some or all of those needs.

 

If you do it right, you only need 1 offset.

[huskermcdoogle]

By G code, yes, by Mastercam... I wish.

 

I think it would be awesome if you guys did a course for this, as I can't find any other training for it. Would you guys modify each users post processor then? Stock Mpmaster lacks some functionality that would be necessary.

 

Last I knew the MPMaster does horizontals and transforms very well....

[Sticky]

If you do it right, you only need 1 offset.

 

Works fine if you are working with parts with loose tolerances, that can be located at the same position every load. For everything else its not so good.

 

Last I knew the MPMaster does horizontals and transforms very well....

 

It works fine if you want one offset for the entire program, or one offset per face. It does not work well for multiple offsets, or multiple parts.

 

http://www.emastercam.com/board/index.php?showtopic=76406

[CJep]

It works fine if you want one offset for the entire program, or one offset per face. It does not work well for multiple offsets, or multiple parts.

 

Is this what you're looking for?

 

N20 G00 G17 G90 G54.1 P1 B0. X.0828 Y1.8413 S5600 M03

N25 G43 H4 Z1.5

N30 Z.25

N35 Z.125

N40 G94 G01 Z-2.5 F50.

N45 X.3259 Y1.5983

**** Code ****

N145 G01 X.79 Y1.8413

N150 Z-2.375 F100.

N155 G00 Z.25

N160 G54.1 P2 X.0828 Y1.8413 Z.25

N165 Z.125

N170 G01 Z-2.5 F50.

**** Code ****

N275 G01 X.79 Y1.8413

N280 Z-2.375 F100.

N285 G00 Z.25

N290 Z1.5

N295 G91 G28 Z0.

N300 G00 G90 G54.1 P3 B90. X.0828 Y1.8413

N305 G43 H4 Z1.5

N310 Z.25

N315 Z.125

N320 G01 Z-2.5 F50.

**** Code ****

N425 G01 X.79 Y1.8413

N430 Z-2.375 F100.

N435 G00 Z.25

N440 G54.1 P4 X.0828 Y1.8413 Z.25

N445 Z.125

N450 G01 Z-2.5 F50.

**** Code ****

N555 G01 X.79 Y1.8413

N560 Z-2.375 F100.

N565 G00 Z.25

N570 Z1.5

N575 G91 G28 Z0.

N580 G00 G90 G54.1 P5 B180. X.0828 Y1.8413

N585 G43 H4 Z1.5

N590 Z.25

N595 Z.125

N600 G01 Z-2.5 F50.

**** Code ****

N705 G01 X.79 Y1.8413

N710 Z-2.375 F100.

N715 G00 Z.25

N720 G54.1 P6 X.0828 Y1.8413 Z.25

N725 Z.125

N730 G01 Z-2.5 F50.

**** Code ****

N840 Z-2.375 F100.

N845 G00 Z.25

N850 Z1.5

N855 G91 G28 Z0.

N860 G00 G90 G54.1 P7 B270. X.0828 Y1.8413

N865 G43 H4 Z1.5

N870 Z.25

N875 Z.125

N880 G01 Z-2.5 F50.

N885 X.3259 Y1.5983

**** Code ****

N985 G01 X.79 Y1.8413

N990 Z-2.375 F100.

N995 G00 Z.25

N1000 G54.1 P8 X.0828 Y1.8413 Z.25

N1005 Z.125

N1010 G01 Z-2.5 F50.

**** Code ****

N1120 Z-2.375 F100.

N1125 G00 Z.25

N1130 Z1.5

N1135 M05

N1140 G91 G28 Z0.

N1145 G28 Y0. B0.

N1150 G90

N1155 M30

%

[guitar]

Works fine if you are working with parts with loose tolerances, that can be located at the same position every load. For everything else its not so good.

 

 

 

It works fine if you want one offset for the entire program, or one offset per face. It does not work well for multiple offsets, or multiple parts.

 

http://www.emasterca...showtopic=76406

 

On the contrary. You can use G54 for all of your faces. Our machine repeats within .001". Anything that needs to be closer can be tweaked with your system variables and macro variables with the WC shift for each face and then cleared after that face's process is complete. Yes, it DOES work for multiple parts.