Haas UMC-750 Post

[kblackwell]

If you are wondering what the point of this post is go here http://forums.autodesk.com/t5/post-processors/sharing-modified-post-processors/m-p/6471708#M10625

This is a post that i have modified for the Haas UMC-750.  It is based off of the generic post included with HSMWorks.  I have included some features from other posts and when I figure out where I got them from I'll edit this post to include references to those.  The features are as follows:

1. I had an issue with the generic post not having the G254 rotation command on the lines after every B or C axis rotation command so i have added that.
2. This post sends the machine to the upper limit in Z every time the B and C axis rotate.
3. This post sends the machine to the upper limit limit in Z and back to the far back left corner of the machine every time the program changes tools (for clearance).
4. I added an option to run the tool probe cycle to touch off only the tools used in the program. ( I got this from another post I'll give reference when i find it).
5. I added an addition to the tool probe touch off routine from #4.  Originally it would not touch off face mills correctly so i added an "if" statement so when a face mill is used it runs two routines, first it runs the normal probe touch off to set a rough length, then uses the tool length from the previous probe cycle and the face mill diameter pulled from HSMWorks tool library to run the face mill probe cycle.  So far everything works perfectly.

I have attached the latest post and an example program.  This program basically just faces, drills, deburrs, and thread mills a few holes.

Haas UMC-750 wTCP-3-25-2016.cps

Haas UMC-750 wTCP-3-25-2016-Output.nc

[cj.abraham]

Could you elaborate on the G254 problem? The post is supposed to output any time the BC axes change unless the BC angles are zero. If the angles are zero, G254 is not supposed to be commanded.

EDIT: The post you've provided is seems to be based off an older version. Many of the points you've made have been fixed, and properties have been added for optionally measure tools, force home on axes positioning, maximum Z retract options. The G254 interaction has also been fixed. I will look closer at point #5, though.

[kblackwell]

@cj.abraham You are correct this is based off an older version of the UMC Post.  Since i had been over 2 years since I originally had this issue it took me a while to nail down what the exact problem was with point #1.  I found the original post processor given to me when i was evaluating the software in 2013 and the only difference i could find is I removed the G255 from the end of every operation and only have it at the end of the program.  For whatever reason this created a problem canceling the rotation command after every operation, our machine has the scars to prove it.  It's possible this was operator related issue but ever since i made this change i have not had the same issue since.  I made an edit to the original idea post to reflect this.

[kblackwell]

For some reason it wont let  me edit the original post so it should read as follows:

 I removed the G255 from the end of every operation and only have it at the end of the program.  For whatever reason this created a problem canceling the rotation command after every operation.  It's possible this was operator related issue but ever after I made this change i have not had the same issue since.  

[al.whatmough]

@Anonymous it looks like 4 out of the 5 ideas on here are implemented. I am going to mark this idea as implemented. And create a new one for idea #5 It looks like a reasonable idea! I will let @Anonymous.Abraham confirm. Thank you for you contributions to the community! Cheers, Al

[kblackwell]

One thing i negelcted to mention, For this to work as good as it does i have modified the sub program for the probe cycle.  I added an M0 to stop the program after the probe cycle changes tools.  Doing this makes it so you can add and change tools as you need.  

When you setup a new job:

1. Load a new program as normal.
2. Turn off block skip, so the tool probe cycle is run.
3. When the probe cycle changes tools there will be a program stop after every tool.  
4. Operator will verify this is the correct tool called out by the setup sheet.
5. If the tool is correct don't do anything just hit cycle start to continue, but if it's not the correct tool they will put the machine in manual, take the tool out of the spindle, install the correct tool, put the machine back in auto, hit cycle start and the machine will continue along the the probe cycle probing the tool you just put in.
6. Continue doing this for every tool in the program.
7. After you are done probing tools, turn block skip back on so the next cycle doesn't repeat this process.

I will upload the probe cycle monday so you can see the changes i have made.

[kblackwell]

For some reason i can't upload the file.  What am i doing wrong, i don't have any options to edit this post, i can only add comments.

[al.whatmough]

@kblackwell you can't edit posts.  E-mail to me al.whatmough at Autodesk  and I will update the request.

[bob.schultz]

As mentioned by @al.whatmough, the requests for 1-3 have already been added to the post.  The post attached to the original request is an older version of the post processor.  Here is the status of your requests in the current version of the haas umc-750 post processor.

1. I had an issue with the generic post not having the G254 rotation command on the lines after every B or C axis rotation command so i have added that.  Already supported in the post.
2. This post sends the machine to the upper limit in Z every time the B and C axis rotate. The existing useMaximumMachineZRetract property can be set to true to activate this feature.
3. This post sends the machine to the upper limit limit in Z and back to the far back left corner of the machine every time the program changes tools (for clearance). Enable the forceHomeOnIndexing property to use this feature.
4. I added an option to run the tool probe cycle to touch off only the tools used in the program. ( I got this from another post I'll give reference when i find it). Added the property optionallyMeasureToolsAtStart parameter to measure the tools at the start of the program.  I discussed the probing Macros with an engineer here at Autodesk and the format is a bit different than in your post, so please test this feature and see if it works on your machine.  Two styles of tool measurement have actually been implemented.  The active method uses the P9023 style of probing Macros.  You can change the conditional in the writeToolMeasureBlock to use the P9995 style instead.
5. I added an addition to the tool probe touch off routine from #4.  Originally it would not touch off face mills correctly so i added an "if" statement so when a face mill is used it runs two routines, first it runs the normal probe touch off to set a rough length, then uses the tool length from the previous probe cycle and the face mill diameter pulled from HSMWorks tool library to run the face mill probe cycle.  So far everything works perfectly. Refer to #4.

One other feature added is the rotary axes will now position to 0 and the machine moved to its home position when checking for tool breakage.