Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Min pass length

9 REPLIES 9
Reply
Message 1 of 10
Jimmy
189 Views, 9 Replies

Min pass length

It would be nice if tool paths like scallop had the option to set a minimum pass length somehow. I know this could all be done with trim, but that could potentially be avoided. On parts with more organic shapes I notice what's going on in the image below happens a lot especially when do not touch surfaces are selected. 

Jimmy_0-1677279316465.png

 

9 REPLIES 9
Message 2 of 10
seth.madore
in reply to: Jimmy

Machining segments like this can typically be avoided with the right combination of Tolerance and "Additional Offset" applied. I typically will have a .0001" tolerance and a -.0002 "Additional Offset" (geometry tab) and don't see those all too often. 

If that doesn't solve your issue, could you share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d file in your reply


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 10
Jimmy
in reply to: seth.madore

This isn't a file I'm at liberty to share. I've tried many combinations of tolerance and offset. FYI surface clearance does more to change this than either of those. But to get it to a point that I would deem acceptable surface clearance has to be around 0.01", which from an finish standpoint is pretty bad. Offset doesn't really do anything since it's set to tool outside boundary. I suspect that tool orientation is more of a contributing factor than anything else, but that's fixed because of clearance. Changing the tolerance can decrease the occurrence of those passes in that one particular location, but actually created more in another spot. I would guess that if the tolerance could actually be zero it would do it, but small tolerances make for a large program size, which isn't necessarily desirable. For some reason turning contact point boundary on and off has an impact on this even though the portions of the tool path that are problematic aren't near one of those boundaries. It's significantly better with contact point boundary on, but still has random extremely short passes. So at the end of the day having a feature where you could automatically get rid of any passes less than a set length would be extremely useful. Not just for scallops too. 

Jimmy_0-1677518596001.png

Jimmy_1-1677518622473.png

 

 

Message 4 of 10
seth.madore
in reply to: Jimmy

Can you share the file privately with me? We respect our customers data privacy rigorously.

If you can't do that (it's understandable), can you recreate the issue in a sample file? 


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 10
Jimmy
in reply to: seth.madore

When I get a chance I'll model up something that replicates this. I'm not really looking for a solution to this so much as requesting a feature. Currently the only thing that solves it is contact boundary on, surface clearance for avoid touch surfaces set to default of 0.0002" or larger, and then using the trim tool to get rid of the handful of passes that don't make sense.

Message 6 of 10
seth.madore
in reply to: Jimmy

While I do understand that you're asking for a new feature as opposed to a solution, the reality is this;

New features (to legacy toolpaths) are often seriously considered mostly when no other option exists to solve the issue. If there's no workflow that produces desirable results, than the chances are much greater that we can make a case for why toolpath "X" needs feature "Y"


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 10
programming2C78B
in reply to: Jimmy

I find making the top height just slightly below the actual top of the feature elimates these, or switch to something like Ramp 

You also get these curlicue/pigtails when doing adaptive inside of a perfectly round bore. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 8 of 10
Jimmy
in reply to: seth.madore

The simplest way to do it would be updating the trim tool to allow automatically selecting all paths less than a certain length. That would save a ton of wasted clicking. A workflow that produces desirable results but takes a long time is inherently undesirable when time is money. The trim tool is especially inefficient because if  I update the machining all those manually selected passes are different and have to be redone. That's better than watching a machine waste time and shake itself apart trying to do a bunch of tiny passes, but that doesn't mean it's good.

Message 9 of 10
programming2C78B
in reply to: Jimmy

I believe you can Trim using a sketch as well, which would stay the same. You can do a projection of the part OD then apply an offset of 1/2 your tool Dia or whatever works. 

Please click "Accept Solution" if what I wrote solved your issue!
Message 10 of 10
Jimmy
in reply to: programming2C78B

There's other parts of the operation where the tool center is about 3mm outside of the edge of the part to wrap around fillets. What you're describing is similar to using the boundary option in the trim feature. It would work if the part wasn't a weird organic shape. But projections end up looping around behind portions of the part that should be machined. 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report