[rockswellwothrs]

I need a hint/ push in the right direction for setting up the "Insert Post Processor Commands". As of right now when listing a 90 deg turn in the drop down menu for rotary table 4th axis i get this [ROTABL/ATANGL,90,CLW,NEXT,ROTREF]. Is this even recognizable to a fanuc control? Is there an area where this syntax can be assigned to macros? If you have any experience with this is there a manual or any reading; I know there is surfcams manual which is chocked full of this stuff, but under which directory would I find this?

[Chrliev]

Nothing in SurfCam is recognizable to a Fanuc or any other controller, thats the job of the PostProcessor, SurfCAM which can be considered the processor doesn't create machine readable output, that's why the Gods (or someone) created post processors.

Before getting all caught up in that, first consider why you would want to do a 90 degree uncontrolled rotation of the machines rotary table..?

The command that you refer to is an SPOST command, meaning it happens only in the post-processor, it does not effect your on screen tool path or your geometry on the screen in SurfCAM in any way, in fact you will only see the results of this command after post-processing your file to CNC code, SurfCam has no idea this command moved your rotary table, actually SurfCam knows nothing about rotary tables, it deals with points and vectors only. The interpretation of the points and vectors is handled by the post...

In general these so called PostProcessor statements are rarely used and only for things like loading/unloading or positioning the machine before and/or after machining. Like maybe you need to rotate 90 degrees for tool changes for a tall fixture or rotate 180 degrees to stop and check a dimension while in a machining process.

As for bathroom reading materials and/or manuals try the SPOST manual...

I hope that gives you the push you were looking for...(wedge)

[Anders6612]

Click the ? mark on the upper right in menu, and then
klick desired button you have questions about.
Surfcam leads you to the answers.

[rockswellwothrs]

thank for the replies.

I guess i didn't mention that the line
[ROTABL/ATANGL,90,CLW,NEXT,ROTREF]
was spit out by the post processor after i had selected the appropriate fields in the Insert Post Processor Commands field for creating a tool path.

And was wondering if I could assign these variables in the PostLib as actual macros that would be readable for the Fanuc control?

My end goal is to be able to program a part with all offset and rotation changes all ready in the program.

I know that I'm going to be doing a lot more work on my post processor but this is the first step.

I'm trying to eliminate hand coding (stitching) the programs together to be able to save tool changes and my nerves.

I feel this is a doable project that will reward greatly in efficiently and stability if done correctly .

P.S. we are as of now using the M Post should I look into the S Post for this kind of customization?

:withstupi

[Camfather]

thank for the replies.
P.S. we are as of now using the M Post should I look into the S Post for this kind of customization?

:withstupi

Spost is more flexible and powerful but more complex to customize (I hope your familar with FORTRAN.

The Mpost that comes with surfcam is good, but it's the "light" version of ground supports PostHaste (Posthaste post processor (Home_) Which is much much more powerful, up to and beyond 5x yet still just as easy to use as Mpost.

Problem is, it will set set you back around $1500

[mariojl]

thank for the replies.

I guess i didn't mention that the line
[ROTABL/ATANGL,90,CLW,NEXT,ROTREF]
was spit out by the post processor ...
:withstupi

Of course it's there, you've asked the Mpost to do so, and as mentioned before, no control will understand it.
May I suggest you to use the “transform” utility in the Operations Manager instead of working on the Mpost??. There you have a powerful tool that will allow to either rotate or index a toolpath.
Also has the ability to “sort toolpath by tool”, letting you select whether change tool or move to a new angle.
You can backplot or edit the toolpath and check in the screen what has been done, and even verify it; and just then postprocess it and send it to your CNC, being sure of a well done job.
This way you’ll avoid any possible mistake. You can merge several programs together with no need to stitch them.
Will have all your offsets and tool changes in the right places and only were you want them. I can assure you that your light Mpost will do want it knows to do.
On the other hand, Spost is newer and more powerful, but it doesn’t make miracles, you have to supply all the info, and this also is done by transforming the toolpath, so it’s imbibed in the *inc file.
Kind regards
Mario

[Chrliev]

thank for the replies.


My end goal is to be able to program a part with all offset and rotation changes all ready in the program.

:withstupi

Believe it or not, that is also my goal everytime that I write a program, 2 axis, 3 axis, 4 axis or 5 axis. I think it is every programmers goal to have all offsets, toolchanges and rotation done in the program, without any editing or stitching of program pieces. My programs go straight from the computer to the machine.

In 25 years of programming I think I have used "insert postprocessor commands" maybe once. My programs run "clean" without doing any of what you believe to be necessary to have a perfect postprocessor. I have tried to explain previously as have others, that this is already done for you using SurfCam itself and the postprocessor as is or with some minor modifications (you might want to re-read and try to understand the replies above).

Having written and coded many post processors for all types of machines in my many years as a programmer and reading your questions above, I don't believe that you have a fundamental understanding of how a postprocessor works, what it does or how it does it. Causing you to totally 'OverThink' the whole postprocessing thing.

I would recommend taking some classes or working closely with someone who has a lot of real world experience writing and using multi-axis postprocessors.

CV