Under Cutting for Thread Mill

[jgiacchi]

Hello,

   I am attempting to figure out how to perform an undercut before I perform a thread milling operation so that I can relieve the bottom of the hole and allow full thread engagement of the screw.  The thread is 8-32, so I use a starter drill bit, then a #29 drill, then the attempted undercut operation for a diameter to 0.164 from the depth -0.22 to -.55 from the model top, then a thread mill from 0 to -0.23 depth.

   I am having two points of difficulty:

   While looking at tutorials and troubleshooting i had to utilize a negative stock to leave in order to have it create the profile and I am not sure why?  Do I need to offset the size of the undercut in the model and then calculate the difference with the negative stock to leave?  That just seems counter intuitive and I am not sure that I am understanding the process flow correctly.

   I can get a toolpath to successfully generate that will perform the undercut, but when the tool retracts it does not return to the center of the hole and will have a collision with the stock.  How to I adjust the retraction so that it avoids the walls?

   I tried various different toolpaths such as 2d Contour, 2d Adaptive, 3d Contour and 3d Adaptive, but 3d Adaptive was the closest I could get to what I was attempting to accomplish.

Any assistance anyone could provide would be much appreciated.  I am also sure I have probably left something off, so let me know what other details you might need,

Thanks,

Jim

[Anonymous · Accepted solution]

Try Bore, given the size of tool and hole, you may want to take more conservative approach on chip load, I adjusted tool parameters to suggest potential solution, "return to center" is key to clearing the wall.

[Richard.stubley · Accepted solution]

Hi @jgiacchi,

I tend to use circular with Lead to centre ticked for times like this.

[Richard.stubley]

@Anonymous sorry, just seen you beat me to this one 🙂

[jgiacchi]

Thank you so much!  This is almost perfect.

As for chipload, I used HSM Advisor to figure it out.  As I was playing with so many things I may not have put the correct speeds and feeds in when I posted the file, but I was planning on using a .125 Diameter Cutter with a .25 Length of Cut.  The Width of Cut will be 0.014 and the feed will be 2.66 IPM.  That should be pretty gentle on the tool at 0.00026 in, I am almost worried I may get some rubbing, but we will see how it works.  If you have any suggestions though I am all ears.

One thing I have noticed is Fusion likes to fully retract the tool in between passes if you attempt to do multiple passes.  Is there a way to change that so it stays at depth and does each pass?  I've noticed a similar behavior for the threadmill as well and it seems to waste a lot of time with movements up and down.  My machine is a Tormach 1100 so it's rapids are rather anemic.  If possible I'd like it to not fully retract, even a partial retract if it needs to clear chips would save a lot of time.

Thanks again!

Jim

[Anonymous · Accepted solution]

There is no option to keep the tool down in thread milling but you can edit resulting code, although with such a small diameter hole you may be better off retracting after each pass to flush the chips out.