Post processing is a critical part of any CAM system, and one that many CAM users don’t know how to manipulate effectively. Join our CAMWorks Technical Expert, Daniel Lyon, for an in-depth look at how you can customize your post processor to optimize machining performance and prevent costly mistakes and rework. You will learn how to create your own CAMWorks post processor using the Universal Post Generator and EC Editor and witness how the different post files interact with each other. Watch this webinar recording to dive under-the-covers of CAMWorks Post-processing and take control of your machining.
Hi Daniel,
My name is Mike Payne and I work at Prop Shaft Supply. Hawkridge is currently our CamWorks distributor. We are in the process of purchasing a CNC horizontal machining center and will need a post. I have been fortunate to so far to use some of the generic post that UPG provides and work with them to build post for our vertical machining centers. The machine we want to by is Okuma MX-40HA with a OSP platform. I didn’t see any Okuma layouts in the standard UPG processor tool. Is there a way to get one for this machine? Also, I was wondering if Hawkridge offered any courses or training for working with and creating CNC post?
Hi Mike,
I am now customizing my own post processor and I am trying to figure out the system command ‘TRANSFORM’
I hope you can give me an example for helping me to understand how this system command work.
another question is in my understanding in the KIN. file Rotation Axis Base Point is for setting offset for C or A axis
but I can not see any differences in GCODE after I change the number
I am doing for my graduation project I hope some one can help me thanks
Hi Mike,
There are a few options available to you for post processors.
1, There is an Okuma OSP post in the standard post processors that are included when you install camworks. The source files for these are in the following location, assuming you used the default install location for the UPG:
C:\CAMWorksData\UPG-2\SampleSourceFiles\Mill\Okuma
2, There is an Okuma OSP300 mill post on our website that is free to download. These posts have a lot of customization included already. You can find these at the following location:
https://hawkridgesys.com/products/cam/post-processors
3, We can certainly build a post processor for you that is customized to your exact machine and to suit your preferences. If this is something you’re interested in, please use the Get a Custom Post option at the top of the post page (the link above) and we can get that process going for you.
Regarding the training courses for building post processors, at this moment in time we don’t have a course on creating and editing post processors.
Hi Fitz,
There are a couple of examples of the implementation of the TRANSFORM function in the UPG>Help>Complete Reference guide under the Transform section. As the help file suggests, the transform function is specific to machines that require the switching between machine coordinates and world coordinates ie it is only in world coordinates for the initial positioning moves and then switches back to machine coordinates until it needs to reposition. You would need to create a CALC section that gets called at the initial preposition call and add the transform variables so that it correctly calculates the transformed XYZ values based on the angle that the machine is at.
If you just need the machine to post out code in world coordinates and not switch between world and machine coordinates you can ignore the above and you can set the flag at the top of the SRC file for :WORLD_POSITIONING=TRUE. For example a simple drill operation on the top of the part would output in Z and a hole in the side of the part would drill in X or Y. You can see this header in the UPG>Fanuc>Generic 5 axis World Coordinate Output. You will see changing the tool protrusion or holder length will affect the g-code output. In this situation you have to be sure your tooling lengths are setup accurately otherwise you may have a crash.
The KIN file is specifically for multiaxis operations and will not affect pre-positioning (unless you have the transform setup to look at the KIN file values) so be sure to test with a Multiaxis Mill operation. You will also need to ensure that the 5 axis type flag at the top of the KIN file is set appropriately. It would have to have no tool comp set to have the code use the rotation axis base points. If it is set to have tool comp the machine is assumed to have TCPC and coordinates are output through the tip of the tool.
Hello Daniel, Just to had a few things to what you repplied to Fitz, if you go for the :WORLD_POSITIONING=TRUE yo need to be a bit careful since there are a few instances that may result in a crash of the machine that come with this option. One is if you are using a tool and change the setup and use the same tool the Z value most of the time will go to an absolute z end and not repositon on where you want so you may need to create a a section to pre position the tool safely. The other issue you may thing is doing is regarding drilling since canned cycles are not going to be used you need to get the sections world drilling from the tutorial post and make some changes to get the drilling in the correct place and if you have multiples drilling with the same tool in diferent setups as well as the peckings. If anyone needs any help i have 4+ years of doing posts for CAMWorks and SOLIDWORKS CAM
Best Regards
André Cardoso