Trace toolpath problem with feedrate

[Anonymous]

Working on a sample milling project for a 2011 Haas MM2 using white Delrin. I have created a simple model with a pocket; island boss; and text. First issue was to find Feeds and Speeds for the material. I found a few posts on the Practical Machinist forum and used those specs as I understood them.

Therein lies the problem. Full disclosure: I am totally new to both Fusion 360 AND to machining in general. I have to reason out the options and formulas so get errors at the mill. First was a 309 error which I attributed to incorrect speed in the post process options. Got that solved. Now my code throws a 320 error, something like "No feedrate set," for the trace process.

I can see that in the g code output but can't see where (or what) to change in the set up tabs. Can someone point me in the right direction? File is attached.

[LibertyMachine]

It appears that the stock post has an error in it. If you go to http://cam.autodesk.com/posts/ and search for Haas (pre-NGC) posts, download that one and it will work

@AchimN what is the update cycle on "built-in" posts

[Anonymous]

Thanks for the reply @LibertyMachine  gonna head over to Haas website right now. Looking forward to trying your suggestion at the mill and will post my result tomorrow!

One more thing. Any chance you looked at my F&S? I am curious if I have things set reasonably.

[LibertyMachine]

Shouldn't need to head to the Haas website, just the Autodesk post website.

Delrin cuts like butter. It does generate a fair amount of heat (through friction), so you want to be using very sharp tooling (carbide or HSS) and coolant. Your speeds and feeds are waaaaay low. What is max spindle speed? For engraving I'd probably run it around 8-10k with a feedrate of 20-30 ipm for starters.

Half inch carbide endmill? I'd be up around 6k rpm with a feedrate of 40ipm or so.

DISCLAIMER!!!!!!!!

You need very secure workholding to make sure the part is not moving around on the table/vise. Delrin (acetal) is quite slippery and jaws will deform it. Clamp it too hard and you can actually bow it enough to pop out of the vise when aggressive machining

A site that I highly recommend for plastic speeds and feeds is: http://www.boedeker.com/fabtip.htm

[Anonymous]

Thank you for the cautions re: Delrin. It will be held in a new, high quality Kurt vise that has been mounted and squared to the table. I am working with my husband who is an experienced fabricator, more to the welding side. He has machining experience on a classic Bridgeport and will be safely securing the material. For my part, the CNC process, I am obviously still in the learning stage so really appreciate your tips and advice. Just what I was hoping for.

I uploaded the Haas post to MyCloud assets as noted. Changed my F&S close to suggested. Posted the new processes and still not getting a feedrate in the g code for the full trace toolpath. As a workaround, I can manually set the lines showing ....F.0 to ...F.20. In my world (programming background) that would be fine but...-- is that OK for mill work??? I'm anxious to see the my practice piece cut while I'm researching the why of the problem.

g code file attached, issue beginning at line N4833

[LibertyMachine]

I'll be a son of a gun. You know what happened? I downloaded the one I indicated and then when I went to post, I missed that it was still posting out a F0..

This actually appears to be a bug in Fusion, as none of my posts are giving a feedrate as well....

Yes, you can perform a CTRL+H and replace F0. with F20.

@jeff.pek @cj.abraham @fonsecr we seem to have a problem.....

Sorry for the confusion here....

[fonsecr]

Thanks Seth. We will investigate it.

[angelo.juras]

@Anonymous @LibertyMachine Thank you for bringing this to our attention. We will look into this.

[Anonymous]

It was making ME buggy so happy there might be a solution coming. 🙂

[Anonymous]

It was making ME buggy so happy there might be a solution coming.

[LibertyMachine · Accepted solution]

Problem found. It's because the tool is defined as a "Drill". If you reclassify it as a chamfer tool you will have additional feedrate options.

@fonsecr seems like it should have failed if a drill was selected.  "Invalid Tool" or persisted in offering cutting feedrate fields

[angelo.juras]

I was actually just looking at it and saw it was defined as a "drill". 

[Anonymous]

Eureka!!!! That was it.I changed the tool and code looks great. We'll see how it goes on the next step.

This is a steep learning curve for me, and the aha moments are especially satisfying. Thank you for sticking with me to make that happen. I'm sure I'll have more questions in the time to come, and truly appreciate the quick responses here.

[angelo.juras]

@Anonymous We will be adding a warning if the wrong tool type is selected in a future release.