3D surfacing tool path not producing arcs - HELP

[geraldAAQ4U]

I'm programming CNC milling in fusion and I'm using 3D contour and 3D ramp and I can't get Fusion 360 to create arc tooth paths.  It keeps creating small linear moves.  I've messed with smoothing and tolerances to see if I could force it to create arcs and I just can't get it to work.  The part I'm machining is a circular boss with draft.  I have to use a surfacing tooth path because of the draft.  The model is imported from CREO as a solid STP file.  I've recreated the boss with draft in fusion to see if it was something to do with my imported STP file and the same thing happens when I program a 3D contour and 3D ramp.  I originally thought it was my post for my Hass TM2P but I started to look at the tooth path data within fusion and noticed they were linear moves, not arcs.

Any help would be greatly appreciated!  I really just want smooth surfaces!   

[a.laasW8M6T]

Ramp cannot ever make arcs as its always moving down in all three axes.

3D contour will make arcs no problems however if you turn smoothing on, there will be line segments on the transitions between passes though, unless you change the transition type to no contact

Ive attached an example file that shows both types

[geraldAAQ4U]

Thanks for the input!  I just created a 3D contour with no contact and no smoothing and it is still producing linear segments.  Just curious if I'm missing something on the path setup or if the STP file output isn't correct. 

[a.laasW8M6T]

There maybe something in the file that is causing issues.

Can you upload it here so we can have a look?(Preferably the .f3d with your current attempts)

[geraldAAQ4U]

For some reason my contours aren't outputting arc toolpaths like yours is. I looked through your file and I updated mine to mimic yours. My file is attached.

[geraldAAQ4U]

Attached below on the next post. Thanks for taking a look!

[a.laasW8M6T]

Hey so there's a few wee tricks to get a good toolpath

1st you need to right click on the toolpath and select "Compare and edit"

then find the surface triangulation tolerance and set it to "tolerance*0.05"

This increases the accuracy of the underlying mesh that the toolpath is calculated off.

2nd, you need to put - tolerance in the "additional offset" of the toolpath boundary

This stops some of the funny whisper cuts near the boundary.

I also found I had to select the center surface as an avoid surface to clean up the path in the middle..

If you turn on points in the toolpath visibility you can see it has a pretty nice toolpath now.

I notice you have alot of NC programs in the browser. If you uncheck "create in browser" in the NC program window you will get rid of that problem.

[geraldAAQ4U]

This is great! I tried this on a couple other tool paths and it worked out. The program started to output arcs! Thank you for looking at this for me! I've been trying a lot of different things to see if I could get it to work. I never knew about the Compare and Edit on the tool path. Is there a universal setting that I can change that would allow all tool paths to use a finer tolerance on the mesh?

[geraldAAQ4U]

Now I have another problem.  I'm getting I0 J0 in my tool path code which my machine errors out on.  Are there any tricks to getting those out of the code?

[a.laasW8M6T]

Hi, Unfortunatly there is no global setting to change the surface triangulation tolerance.

But you can go into each of the toolpaths you want to change it and then set as default:

as for the arc problem, there may be a setting in the NC Program window to change to radius arcs rather than IJK

[geraldAAQ4U]

I figured out that I had my tolerance and smoothing tolerance tool low. It was still putting out zero radius arcs or close to it. My TM2P didn't like those. I ended up increased the tolerance until it gave me a small radius. Thanks for the help!