Same post, but output code is different between version 8.1 and X2

[MILLRUNNER]

I have a situation I'm trying to resolve. I have an old Hitachi wire EDM machine which has a fanuc control and it has been programmed with 8.1 for years. I have recently learned and use X2, and I am going to have to start programming from X2 to this particular machine.

 

I can do everything in X2 that I can do in 8, same sequence, same everything, but when I post the code it comes out totally different between the two versions.

 

This is a simple 1" x 1" part with a .5" hole in it.

 

Version 8.1 code:

 

O100

N100 G90 G95

N102 G92 X0. Y0.

N104 G00 X3.99235 Y1.72491

N106 / M00 (THREAD WIRE)

N108 G92 X3.99235 Y1.72491

N110 G01 G41 X4.24235

N112 G03 X4.23989 Y1.68991 I-.25 J-0.

N114 M00

N116 G50 X4.24235 Y1.72491 I-.24754 J.035

N118 G01 G40 X3.99235

N120 / M00 (CUT WIRE)

N122 M30

%

 

---------------------------------------------------------

 

Version X2 code:

 

O1 N100 G90 G95 N100 G92 X0. Y0. N100 G00 X0. Y0.

N110 M82

N120 M81

N130 M60

N140 G92 X0. Y0. N140 G01 G41 X.25

N150 G03 X.24754 Y-.035 I-.25 J0.

N160 M00

N170 G50 X.25 Y0. I-.24754 J.035

N180 G01 G40 X0.

N190 M50

N200 M21

N210 M42

N220 M41

N230 M30

 

---------------------------------------------------------------

 

I updated the post through X2 and I am in that post when I draw my geometry.

 

Any help would be appreciated.

[K2csq7]

If your up for it (at minimum a few hrs work), your going to have to use the post debugger to find where the output is coming from in the post, then alter the post (always back up first) to make it do what you want. If your not up for it, your going to have to go back to your reseller....

There were some changes to the post format when X came in, just running the "update post" wont do everything you need it to, maybe your reseller can take a quick look and make a couple minor changes for you.

If your in the mood to do it yourself, I would suggest starting with a fresh copy of mpmaster...

[MILLRUNNER]

Well I've never edited a post before, and I'm sure there is alot more to it than meets the eye, but I feel like I could do it. I might call the reseller back today and explain the situation to them.

 

All the post does is tell mastercam exactly how to output the code, correct?

[K2csq7]

Yeah, piece of cake....

But seriously if you have the time and motivation go for it, rearranging the code is easy, but it looks like you have some issues with the X & Y #'s, that maybe a bit more in depth...

[Pimp_your_post]

Since you updated from version 8.1 to X2, you now have to deal with machine definition files and control definition files. More specifically, the control definition file has options in there that WILL modify the output of your post. For example, there are settings for your arcs, your feed and there is even a setting that will add spaces in between all your words.

 

When updating to X2, Mastercam should've created these two files with default settings. Problem is, these settings may not be right for you.

 

I would therefore suggest that you take the time to look at all the options available in the control def, play with them and you should be able to regain your proper output.

 

Also, open up your post and search for lines that start with "#CNC". These are lines that have failed to update properly. You will most likely have to fix a few of those from the look of things.

[MILLRUNNER]

So what is mpmaster?

[K2csq7]

Free generic post from inhouse, at the top of this page go to downloads, you will find it

[Paul Decelles]

Old wire posts generally require more work than simply running them through update post to get them to process correctly in X or beyond due to changes in MP processing over the years. I would highly recommend contacting your local reseller for help updating the post, he can always forward it on to us if needed or may have a more modern solution already available. It is unlikely that tinkering with CD settings is magically going to fix the issues I see in your sample code. This line alone: "O1 N100 G90 G95 N100 G92 X0. Y0. N100 G00 X0. Y0." tells me that you are missing e$'s on some post lines and that the rpd_typ_v7$ and tlchng_aft$ variables likely need to be modified which in turn require changes to logic using cstart$ and cend$ flags. The modifications required will take time and some bit of expertise to achieve.

[Jimmy Wakeford from Barefoot CNC]

... a more modern solution already available

 

+1 to what Paul said. The older posts do not take advantage of all the new features in Mastercam.