PLEASE HELP! Chamfer Bug!

[Anonymous]

This morning Fusion updated with the new January 2017 patch and since this update all my chamfers are posting out with a F0. in some of the G1 commands.  (See attached file).

I know it definitely is not the post processor as I was making parts yesterday just fine.  I have heaps of parts to make and simply do not have the time to edit all the F0.'s to the correct values.

Fusion Team, please fix this ASAP!!!!  I am in trouble.

Kind regards

Grant Nicholas

[Steinwerks · Accepted solution]

I'd bet this is because you're using a Drill that doesn't have a feedrate in its definition. Change that to a Chamfer Mill tool defined the same and it should fix it.

[Anonymous]

I bow to your God like powers of deduction!  Kudos added!!!!!!

Thanks so much I do really appreciate it.  Weird thing is how it has always worked till now.......?

Cheers

Grant

[Steinwerks]

Are you using a generic post or a custom one? Is the tool defined as a Spot Drill specifically, or just a Drill but short? Spot Drills, Counter Sinks and Center Drills have cutting feedrates whereas plain drills do not so it could be a definition issue in this case.

[Anonymous]

Generic Tormach Path Pilot Post Processor.

I have always had it setup as a Spot Drill which contains a cutting and ramp feed rate.  It would appear that something has changed as it requires lead in and out feed rates now too????

Cheers

Grant

[Steinwerks]

Would you be willing to Export and share your part file here? I'd like to see what's getting output to see why a Spot Drill isn't working, because it should as best I can tell so far.

Edit: nevermind, I've figured where it's coming from. There is no Lead-in or Lead-out feedrate applied to the Spot Drill and so it defaults to zero. There might be a way to override this in the post, but it's going to be a much safer bet to simply define a Chamfer Mill.

@jeff.pek is there a plan for this? I don't think this is the first time this has come up.

[jeff.pek]

I'll look into this. I can't answer offhand right at the moment.

  Jeff

[Anonymous]

@jeff.pek I have seen that this was a problem in HSM Inventor to about a month ago.  

Will be nice to see a fix for it soon.

Cheers

Grant

[Anonymous]

http://forums.autodesk.com/t5/hsm-support-forum/chamfer-using-drill/td-p/6082006

[onellesen]

Thank goodness this was here, I have hot parts and fusion force updated then that feed issue occurred, changed to chamfer mill not spot drill and Viola!

[Anonymous]

Oh man, I can't tell you how glad I am for finding this post.  I thought I was going crazy.  Changing the tool type to chamfer mill did the trick.  All is right with the world.  Well, my CNC world that is...

Thank you!