Milling round stock from side, cutting lots of air

[jblack]

So I'm trying to mill a round piece from the side, but Featurecam still acts like the stock is square even though I have it set as round? It wouldn't be a huge deal, but it's from stainless so it's wasting a couple of minutes per side just cutting air. 
I've tried using stock model, and importing a curve as stock but it still seems to do the same thing. Is this just something I'll have to live with? I'll attach the file I'm using. 

EDIT: I'm using FeatureCam 2018

[bhorstTGM48]

Inside of FC I created a solid model to represent your stock. Then I went into the feature and set the "Use solid model" to the new solid I created. I believe this will get rid of that air cutting. 

https://www.screencast.com/t/hizojDuTgH5w

[Anonymous]

Hi @jblack,

Use the tip you got from @bhorstTGM48, then you got this result.

[abhishek.juvekar]

Hi @jblack,

Thanks for posting on Autodesk Forum.

Other method is you can create a stock model with reference to the stock, recompute by right clicking it and use it in the Z level rough feature.

I have attached a fm file. Let me know if you have any questions with reards to this toolpath.

Thank You.

[Anonymous]

Hi @abhishek.juvekar,

Yes I agree with you, you can use the stock models to limit the air cutting, but my experience is you increase the calculation time as soon as you use stock models in FeatureCAM, since the stock models dosen't works as in PowerMill.

[jblack]

I tried this, and wound up with the same results. I'll attach the new file, maybe I did something incorrectly?

[jblack]

This does the same thing also. I'll attach a screenshot of what I'm seeing and not desiring to insure I'm saying the right things. In the screenshot, anything outside of the white lines is what I'd like to get rid of. 

Thanks for the replies so far!

[bhorstTGM48]

Yes, your new file is correct. I downloaded it and it works perfect here. Maybe it has something to do with your version 2018? I opened it in 2017 and 2019 and it works perfect in both versions. Absolutely no air cutting.  

[abhishek.juvekar]

Hi @Anonymous,

Agree. It takes time to calculate stock models. However, I wanted to convey it is one of the methods which can be used to generate toolpath with respect to the remaining stock available if user has no problem with its calculation time.

Thank You.

[abhishek.juvekar]

Hi @jblack,

I too found a correct results in 2018.3.4.016 and 2019 with your new fm file as well as my fm file. Refer attached images.

Thank You.

[jblack]

So I went ahead and upgraded to 2019, and I still get the same issue. Is it possible I have something set wrong somewhere that's causing it only on my end?

[abhishek.juvekar]

Hi @jblack,

Can you please try to rename or delete your INI and XML files which are available at C:\ProgramData\FeatureCAM? Make sure to take a backup of those files and let us know the feedback.

Thank You.

[jblack]

Just to clarify, the ezfm_ui files? 

[abhishek.juvekar]

Hi @jblack,

Yes, ezfm_ui files. I am not sure which option is affecting this. Close FeatureCAM, rename or delete these files (MAKE SURE TO TAKE BACKUP OF THEM), reopen FeatureCAM. Then verify again. If that resolves the issue, send those ezfm_ui files to me. I will take a look into it.

Thank You.

[jblack]

This did fix it! I'll attach those files on this message. 

[abhishek.juvekar · Accepted solution]

Hi @jblack,

Thanks for supplying INI and XML files which make me able to reproduce the above behavior.

I verified this issue with your INI and XML files and found that DMK 3D Toolpaths was unchecked in secret menu. If I check it, recompute the stock model, simulate again, it is clipping the toolpath correctly according to the stock model.

Refer a video DMK settings in secret menu affecting surface milling toolpaths.

Note: I verified it with creating a solid model of stock and using it in a Z level > Stock > Use solid model. The same option is affecting it too. If I check DMK 3d toolpaths, created a solid model again and used it in a stock tab, clips the toolpath correctly.

Hope this helps.

Please click on Accept as solution button if my post answers your query.

Thank You.

[jblack]

Thank you @abhishek.juvekar! That looks much better. 
Also thanks to everyone else who took the time to give me suggestions and work on this!