Heres how to add Post Processor Operations to Camworks

I'm using:

Camworks 2001 plus
Solidworks 2001 plus

When I try to use the "Insert Post Operation", there isn't anything listed there.

I was expecting the mandatory and optional stop commands (M00/M01), but those aren't there either.

The Camworks post processor architecture is poorly documented and disorganized. I'm an experienced programmer and this is garbage. I scoured the internet and all I could find were several versions of the same document, which basically just lists all the identifiers, commands, and variables, but doesn't provide an overall picture of the structure.

The files that play a role are:

your_machine.SRC
your_machine.LIB
MILL.LIB
MASTER.ATR

"your_machine" means whatever the filename for your particular machine is.

The above files are all human readable. I'm not going to attempt to "describe" them since they all seem to have similar aspects and its not clear to me what can or cannot go in any of them. And good luck finding any documentation on that.

NOTE: before you try any of this junk you should at least figure out how to edit the relevant files in notepad, compile them using UPG, and then reload your post processor in camworks.

So, here are the steps:

STEP 1: Getting something to appear in the "Insert Post Operation" dialog box.

Add another operation in your_machine.SRC after all the existing operations. It looks like Camworks puts whatever additional operations you add into the Insert Post Operation dialog box.

:OPERID=Option stop
:OPEREND

Add an entry in MASTER.ATR which gives the new operation an "ID", and also update the HIGH_ID number in that file.

:OPERID=Option stop
:ATTRID=17506 <--------- use the next highest ID number above whatever is at the bottom of your MASTER.ATR
:ATTREND

:IDHIGH=17506 <---------- this is at the top of MASTER.ATR. Edit it to make sure its equal to the highest ID in MASTER.ATR

."Option stop" will now appear in the Insert Post Operation dialog box, but it wont do anything.

STEP 2: Getting your new post operation to DO something.

Now lets add what we need to make "Option stop" actually output an M01 in the NC code.

Add a new "SECTION" to MILL.LIB that inserts the M01 code.

find this line in MILL.LIB:

:SECTION=CALC_START_OPERATION

and right after it, put this:

:C: IF OPR_TYPE=OPTION_STOP THEN <-------notice how its all in caps and now has an "_" instead of space? all that matters.
:C: CALL(OPTION_STOP)
:C: CALL(CALC_CHECK_OPER_COMMENTS)
:C: RETURN
:C: ENDIF

Next, add a new "SECTION" that will output the M01 code:

Go to where all the SECTIONS are in your_machine.SRC, and add this somewhere:

:SECTION=OPTION_STOP
:T:M01<EOL>


Now recompile, reload your post processor in camworks, and insert a new post operation. Select the "Option Stop".

Now post process, and look at your code. You should see an M01 wherever you inserted the post operation.

Some other things I've learned, that if someone asks I will gladly post instructions for:

How to make it so you can have a list of predefined options to select from when you insert the post operation. I.e. instead of "option stop" it would be "Stop" and the list would have "Mandatory Stop M00" and "Optional Stop M01".

How to make it so on the Post tab of each operation you can enter a value directly or use a list and have it output and/or modify NC code based on that.

IMPORTANT NOTES:

Notice how I called it "option stop" instead of something more logical like "optional stop"? Well it turns out there is already a bunch of "optional stop" "program stop" crap inside all those text files and if you use an existing name and it conflicts it wont work and you'll be wondering why. So either cleanup all the files so they aren't using the names you want to use, or use names that are definitely unique and make sure they arent already in the files.

Also, it seems that you may need to CAPITALIZE and use "_" underscores instead of spaces sometimes even when referring to an identifier that is elsewhere lowercase and with spaces.

Thanks for your information. I'm also trying to figure out how to make things to work about post and API . There are not enough information about these topic and I haven't gotten any response from Geometric.....

Quote:

---

Originally Posted by hoisee

Thanks for your information. I'm also trying to figure out how to make things to work about post and API . There are not enough information about these topic and I haven't gotten any response from Geometric.....

---

What are you trying to do? Be as specific as possible and I might be able to help.

We had just upgraded CAMWorks to 2014 version (from 2001, same as yours ^_^) and are going to have a new 4 axis machine with a prepositioned tilting head (fixed during machining) and two horizontal spindles. This machine will not support coordinate rotation function, so we have to have a new post to handle world coordinate system so that we can transform machining direction into X,Y,Z correctly. Our dealer seems has no ability to handle this so I planed to write this post by myself. I had basically solved this problem just by turning on a parameter in the post. Now, I could output wcs correctly. But I still have no idea about how to handle tool compensation in this tilting head situation.

As to the API, it is the same situation that Geometric didn't provide enough information to the customer so we have to guess the functionality and parameters of their API functions. They claimed in the API documentation that we can contact them if we have questions about API, but I had gotten nothing or maybe they will reply me later. However, I had figured out how to write CAMWorks API. Now, I can have my own add-in in the SolidWorks environment to handle CAMWorks task successfully.

It's glad to see someone also trying to figure out how to master CAMWorks post, but it's sad to Geometric. I miss Teksoft so much.... quick and correct answers.....

Quote:

---

Originally Posted by hoisee

We had just upgraded CAMWorks to 2014 version (from 2001, same as yours ^_^) and are going to have a new 4 axis machine with a prepositioned tilting head (fixed during machining) and two horizontal spindles. This machine will not support coordinate rotation function, so we have to have a new post to handle world coordinate system so that we can transform machining direction into X,Y,Z correctly. Our dealer seems has no ability to handle this so I planed to write this post by myself. I had basically solved this problem just by turning on a parameter in the post. Now, I could output wcs correctly. But I still have no idea about how to handle tool compensation in this tilting head situation.

As to the API, it is the same situation that Geometric didn't provide enough information to the customer so we have to guess the functionality and parameters of their API functions. They claimed in the API documentation that we can contact them if we have questions about API, but I had gotten nothing or maybe they will reply me later. However, I had figured out how to write CAMWorks API. Now, I can have my own add-in in the SolidWorks environment to handle CAMWorks task successfully.

It's glad to see someone also trying to figure out how to master CAMWorks post, but it's sad to Geometric. I miss Teksoft so much.... quick and correct answers.....

---

Hmm it sounds like you've definitely delved deep into this. The stuff I've been focusing on has all been about getting it so I can enter variables inside camworks and have those variables appear in the NC code and/or affect the NC code.

Once the wcs is rotated, why does the tool compensation need to be updated? Do you mean tool length compensation? What happens when you run a program?

Worst case, you could write a new section in the post which does whatever you want and have it execute in place of an existing section.

BTW, do you have any service pack discs for camworks that you'd like to sell? I cant get service packs anymore and as I'm sure you know 2001 has tons of bugs.

I have not spent too much time to research post cause I'm still waiting our reseller to provide us a new post to handle this situation. I just want to make sure that in the worst case I can solve it by myself.
As to tool compensation, yes, I meant tool length compensation cause it is not possible for the new machine to do tool radius compensation in the wcs mode. I think I just need a field to fill in a XYZ shift amount for each tilted tool at that specific tilting angle. I don't know others how to handle this tool length compensation when the spindle is equipped with a manual rotated tilting head. Do you know anything about this?

Our old SolidWorks/CAMWorks 2001 version was upgraded from 2000 version and is older than your 2001 plus version.........
Maybe you can consider upgrade to 2014 cause there are many new features in both SolidWorks and CAMWorks. Many of my concerns in the old version bugs had been solved several years ago. As to CAMWorks, it is very stable and it supports SolidWorks configuration now. Especially, it supports API so that we can do many customizing works. I will spend most time to develop CAMWorks API from now on. Although CAMWorks has the tech DB to facilitate many things but it is still not very automatic... For example, one of my macros will let me to highlight a face then click my CAMWorks command then it will generate the required NC file in the specific directory ( still under construction, but I had proved that it can work). And as you mentioned that you are a programmer, I think you will be very excited that you can customize your CAMWorks. However, the documentation about CAMWorks API is written poorly. No detail parameters usage description, some methods no returning object type.... you have to guess to make it work!

Hi,i need help on a matter and i hope you could answer.


i'm configuring solidworks 2018 cam (it's powered by camworks, it is really the same thing) using camworks universal post configurator.
i'm operating on a FAMUP 120 machine with sinumerik siemens 840D control.
i configured drilling functions using sinumerik modified cycles, it's working.


I want to implement also pocket3 (rectangular), pocket4 (cyrcular) and cycle71 (face mill) in the postprocessing, but i have no clue how it can be done...
Can you help me please?