Engraving on 4th axis with a VMC mill

[Anonymous]

Hello all,

I am attempting to engrave on a cylinder by using a wrap tool path. It will generate the tool path but whenever I post (Fanuc) it tells me that my machining configuration does not support movement. I've discerned that it is looking for a 5 axis post processor which I don't have since I just have a 3 axis machine with a rotary table. My question is, is there another way to go about this with just a 3 axis mill and rotary table? I have tried trace and multi-axis contour but I can not get it to act the way I want. I have attached the file so maybe someone can take a look.

I have also always used the CamWorks font style which I am learning does not seem to work well with wrapping tool paths as it has open contours. Can anyone recommend a better font for this sort of thing? What sort of tool performs best?

If you haven't noticed, I am still a beginner.

Thanks for your help!

Edit: I forgot to mention that I use Solidworks with HSMworks.

[paul.clauss]

Hi @Anonymous 

Thanks for posting! I found that, when using a 4x post processor, the code posted correctly. I used the Tormach PathPilot post with the rotary defined as around Y to test this. The  instructions in this article show how to set up a rotary axis in a post - you'll just change a "true" to "false" in the rotary definition.

The 2D Contour wrapped toolpaths in your file will also work - these will work better if you use a single line font. Solidworks seems to have some single line fonts you could use - please see this article in their learning materials for more information.

I hope this helps! Please let me know if you have questions.

[Anonymous]

Hello Paul,

Thanks for responding! So I realized that my error came about when I tried posting in "Fanuc - Inverse Time - A axis" I got an error "Direction is not supported for machine configuration". This was originally why I started this post.

Now, however, after acting on your advice. I posted with a regular Fanuc post processor without changing the "true" and "false" options. It posted with no errors. Then I posted again with the rotary option set to "true"  with rotation defined around the X axis. It posted again with no errors but the strange thing was that the two posted codes were completely the same. I rechecked the instructions you gave me and I think I followed them correctly.

Any idea as to what the issue is?

[paul.clauss]

Hi @Anonymous 

Thanks for the response. Changing the post property in the "Post Process" dialog should make the change in the post regardless of the true/false setting - I think this is what is happening with the generic Fanuc post. I would expect these posts to be the same. I believe setting the rotary in the post processor actually overrides the true/false settings shown in the post.

I am curious why this is not posting with the Inverse time Fanuc post - I've asked the post team about this problem behavior and will report back.

[paul.clauss]

Hi @Anonymous 

Thanks again for posting! I had a closer look and noticed that this is a setup issue - your setup uses the Y-axis while the A-axis post is set up to rotate around X. The X-axis is the RED axis on the job triad:

Apologies for the confusion here! I hope this helps - please let me know if there are further problems.

[Anonymous]

Well, now I am a little confused because I see your point about the initial setup but if you click on the contour operation, the axes change and the x-axis becomes the rotation axis. I can change it in the initial setup so they are the same. I may have been setting this up wrong the entire time.

When I do post the code, I get a G43.5, which to my understanding is a Fanuc code for Vector programming for 5th axis. My machine will error out whenever it gets to this line. I know this machine supports this type of work because I've done other rotary work before but usually I will post in Inverse Time. Is there a way to only allow for 4 axis posting? I've attached my post processor I'm using so you can try it with mine.

I also do not have an option for setting the rotary in the post processor, as far as I am aware.

[paul.clauss]

Hi @Anonymous 

Thanks for the response! I believe the error at the machine is because you need to use the Fanuc A-axis post - the other will always output IJK vectors. 4-axis machines rarely come with the RTCP/ G43.5 option.

The generic Fanuc post processor is setup to handle any multi-axis configuration and outputs the tool axis vectors (IJK), instead of the rotary angles. So it doesn't really know what type of tables/heads are on the machine and infers a solution. The error at the machine should be resolved with the Fanuc with A-axis - I was able to post this code and received the results below - this was all the 2D Contour toolpaths.

I did notice some odd behavior in the file this time. While tool orientation is not enabled in any of your 2D Contour toolpaths, the operations are being pulled back to the model orientation for some reason. This is what you are seeing and I've logged a defect on this. You can see the correct tool orientation is shown when editing the operation and I believe this is a visual defect - the code seems to be coming out correctly. I've logged internal ticket CAM-14712 on this behavior, thank you for bringing it to my attention.

[Anonymous]

Would it be possible for you to share with me your "Fanuc with A-axis" post processor? The only A-axis processor I have is the "Fanuc - Inverse Time and A-axis" processor. Is this the same? Whenever I post with it I get a post error that states "Direction is not support for machine configuration" and that it "Failed to invoke 'onOpen' in the post configuration". I will attach the log to this reply.

My tool orientation has always done that and I never thought anything of it. It has always worked when I have used inverse time before. Hopefully, it can get rectified!

Edit: I just downloaded the newest version of the Fanuc with A from the autodesk post library and I got the same error.

Edit: I also attached an updated file. I am now using a single line font and have been trying to post from "Job (1)".

[paul.clauss · Accepted solution]

Hi @tyler3J6TX 

Thanks for the response. I'm using the inverse time post as well, apologies if that was unclear. Post linked here.

You will need to fix the setup in your file so the rotational axis is around X instead of Y - I've shown my workflow in the screencast below. I hope this helps.

[Anonymous]

This worked great! I made the appropriate changes and it posted with no issues. Thanks for the video, I think I understand it now. However, How would one get it to post around the Y? Is this even possible? Does it have to be defined in the post processor first?

Again, really thanks for your help!

[paul.clauss]

Hi @Anonymous 

Thanks for the response - I'm glad to hear things are working.

You can certainly use a B-axis with HSM - the post would just need to be set to have the B-axis rotation around Y. Rotary setups within a post are described in detail in this article. After setting up a Y-axis post, you'll just need to be sure that the WCS defined in your job setup is at the center of rotation for the B-axis - just like we did with the A-axis in this thread.