Turning profile retract question

[timothyhinessr]

I'm trying to program a simple roughing profile operation on a cast part that doesn't allow me to approach the start of the cut from outside the material in Z.  To clear the Z positive end of the casting, I have to have my clearance height about 1" away from the surface of the area I need to profile, and have to basically plunge into the part in X before starting my Z move.  Due to the material and shape of the casting, I have to use a very slow RPM and feed rate, .012 IPR and 500 max RPM's.  I have over 100 of these to do and have to make three passes to get to my target OD.  Still pretty new to turning in Fusion, I understand that from the clearance height in X, the X feed rate to the outer radii is the same as the programmed profile cutting feed rate which in my case is .012 IPR.  That being the case, with a 2" cut in Z, and 1" feed in Z, each part will take approximately 13 minutes.  I've spent the last couple of hours trying to find a way to make the 1" move in X from the clearance height to the outer radii faster but cant find a way.  I've tried a couple of different suggestions from AI but couldn't get them to work either.  Any suggestions or am I just stuck with an inch of air cutting at .012 IPR per part?  Thanks in advance, Tim   

[marcus.toepke]

A picture/drawing says more than a thousand words.
Even better would be an *.f3d file!

How is anyone supposed to imagine something from your description?
It's like dowsing. 😉

[timothyhinessr]

Here is the file.  It isn't an accurate representation of the actual shape of the casting but gives you the general idea of what I'm up against. I didn't model the actual shape because it would involve a curved conical shape, like a cow's horn, that I don't see the need to take the time to do for the purpose of this project.  I know the simulation shows the insert rubbing at the beginning of the toolpath but It will clear on the actual part. I hope this helps. 

[timothyhinessr]

I finally found a way to change the speed that the X axis feeds from the clearance plane separately from the operation's programmed feed rate.  Under Linking in the Linking Tab, set the High Feedrate Mode to "Always use high feed".  Leave Rapid to Next Cutting Depth unchecked.  Set the "High Feedrate per Revolution" to whatever feed rate you want.  It appears to default to the feed rate you set in the tool tab for the operation.  For my operation, I changed the High Feedrate per Revolution from .012 IPR to .05 IPR.  While this does speed things up, it does result in the tool feeding into the stock axially at .05 IPR before beginning it's Z move.  It also limits the speed of the move from the end of one tool path to the beginning of the next in multiple depth operations, as well as the retract feed rate at the end of the program to .05 IPR.  Once I got everything dialed in, I was able to cut the machining time for each part in half. So while not optimal, it's way better than when I started.

[seth.madore]

If I'm understanding you correctly, you're not able to position the tool at the actual front of the part, either due to the part being quite long or perhaps you have a tailstock that's in the way. One feature that you might want to investigate is the Approach and Retract settings, where we permit "First/Last Toolpath point". This would give you a toolpath like this:

In regards to your feedrates, there IS the "Angled Entry" option, which gives additional feedrate options for entry. This is found on the Linking tab:

[timothyhinessr]

Thanks Seth, good information.  The problem isn't with not being able to reach where I need to, its not being able to reach it from outside the part in the Z axis, and having to plunge into the stock in X.  I found a solution that works, as my last post describes, but it would really be nice if Fusion turning allowed the same flexibility for approaching the part in X that it does for ops on a mill, that being the ability to set a "plunge" feedrate that stops just above the part where it would then feed into the part at the programmed feedrate. Maybe someday. 

[seth.madore]

I must confess, I'm not following exactly what you're asking/looking for. Any chance you could mock something up with MS Paint or some other screenshot marking tool?

[timothyhinessr]

Seth, this is the part I'm working on.  The red arrows shows the rapid toolpath from home to where the cut has to start (model front).  The blue line shows the X move that I'd like to speed up significantly.  As described above, I can speed this move up, but whatever speed I set it to is the speed that it plunges into the part.  Also, this operation requires three passes at the .012 IPR feed rate.  At the end of each pass, the tool retracts slightly and then "crawls" back to the beginning of the tool path for the next pass.  And finally, after the final pass, the tool retracts slowly in X to the retract height and then slowly in Z, represented by the green line. Once it reaches the model front, it rapids back home.  I may well be missing something obvious due to lack of experience programming turning operations, but it seems there must be ways to speed up all these moves to reduce machining time.   I hope this clarifies what I'm looking for.  I've also attached the file if that helps.  Thanks, Tim     

[timothyhinessr · Accepted solution]

Seth, I finally figured out what I hadn't previously understood about Fusion turning operations.  With a little help from AI, and by studying the G-Code for my operation, I learned that Fusion has an internal non-user exposed parameter called the "Radial Safe Engagement Offset".  This .020" offset, which apparently cannot be changed by a user, automatically causes the tool to stop .020" from the programmed stock to avoid high speed collisions.  From there, the tool feeds at the programmed feed rate, in my case .012 IPR, to the programmed depth of cut before beginning the Z move.  The Radial Safe Engagement Offset works the same regardless of whether your using the "Always use high feed" or "Preserve Rapid Movement" linking setting.  By using the Preserve Rapid Movement mode, and reducing my clearance height as much as safely possible, I've been able to get my machining time for this part down to just under 4 minutes.  So as is not uncommon, my "issue" was my lack of understanding as opposed to a problem with Fusion.  My apologies😉