I would appreciate help understanding parallel toolpath and parameter selection

[t.g.mandel]

I am working on my first 3D carve, and it is my first 2 sided project as well.

All is going well, thanks to the help of forum members.

With a roughing pass successfully completed, I used a parallel toolpath for finishing.

I would like help understanding what it is doing, and the parameters responsible. Here is what I am seeing:

1. The toolpath moves in both directions, which I believe is what I selected

2. The ball nose endmill I am using seems to advance about 1 mm overall  in the Y/cut direction, through a series of about 6 back and forth passes

3. From the sound, it seems to me there is tool engagement on these passes

*4. What happens next I do not understand - the toolpath/endmill seems to now go back the other way in the Y direction, and I do not hear any cutting, and it seems to make more than 6 back and forth passes before it starts advancing and cutting again

I have attached my file, and an image below of the setup. The parallel pass discussed is the one shown in the screenshot below.

Here are the two tabs I think may be of importance:

[seth.madore · Accepted solution]

You have "Machine Steep Areas" selected, with a stepover of .02mm, which is very very very small. You likely won't hear any engagement for quite some time. When it approaches shallower areas, you could see a stepover as large as .4mm. 

You might likely be better served with a Scallop toolpath, as the stepover is going to be a lot more consistent, with the added benefit of a lower cycle time

 

[t.g.mandel]

Thank you for the reply and explanation.

I will try the scallop tool path.

[t.g.mandel]

I wanted to thank you and follow up with an update.

The scallop tool path is indeed the way to go - much faster as well. I was worried that it too closely followed the roughing pass lines, but it finished extremely well. Here are two photos of the work.

I did have one last question I was hoping you could help me with. There were some odd vertical moves at the end of the scallop tool path - at the tail and side - that left some material. See photos below:

I was hoping there is a setting I can adjust so the tool makes clean horizontal passes to remove all these artifacts. I tried to have enough overlap on the top and bottom machining to avoid this. I imagine I can rework the model surfaces, but thought if you had a look at the CAM something simple might be available to modify.

Thank you for your ongoing support.

[HughesTooling · Accepted solution]

How about using Scallop down to the tabs then use 3D Contour to go down just past the centreline. See attached file.

Mark

[t.g.mandel]

Thank you for taking the time to reply and for the suggestion. 

Do you know why when I tried this - going well below the centre line on both top and bottom setup scallop toolpaths - it left the shown material? I am asking to better understand if there are fundamental differences in the way the 3D contour and scallop toolpaths work.

I am still fine tuning the machining of this project, so will try the 3D contour on my next bird. I will share the results when finished.

[HughesTooling]

I'd guess Scallop is struggling to find a clean path around the centreline where the part is virtical and starts to undercut. For virtial areas 3d contour will work better. Always a bit of a compromise where some toolpaths work on flater areas and some virtical.

[t.g.mandel]

It worked very well - the artifacts along the steep sides have been machined away. Here is the top of the next carve where I finished with a contour tool path as you suggested. I think I now have a proven process that provides excellent and repeatable results. Thank you again for the help.