Thread Mill: How to adjust feedrate on arc entry?

[M Ham]

Thread Milling an 8-32 hole. Starting at bottom of hole, "climbing" up. Code looks good, but I would like to apply a slower feedrate to the 1st arc that initially enters the cut. Most thread mill manufacturers will advise a 1/2 feedrate for this initial lead in arc. I have my plunge feedrate set to a slower feedrate than my cutting feedrate, but the plunge feedrate is applying itself to the entry from the straight move to the bottom of the hole.

"Colors" even show the arc entry as a different color noting it's an "entry motion".

QUESTION: How do I apply an alternate feedrate to the entry leadin arc?

Using Mastercam 2023 Update 4.

Thank You.

[David Colin]

You could use toolpath editor to modify every hole. If you have a bunch of holes it will be a lot of work though. 

It probably can be made with a post modification too but it will need post coding knowledge to identify toolpath type and first arc motion.

Looking at your toolpath, you probably use a single point (or profile with 2 or 3) thread mill so I would suggest to conventional mill your holes from top. That way tool will enter the cut progressively and it won t really need to decrease feed. 

[gcode]

I put in an enhancement request for this late last year.

I referenced the Carmex threading wizard which outputs F/2 lead-in feedrates.

My request was way too late for the 2024 development cycle though

[Chally72]

This and some other Thread Mill entry capabilities are currently in the works, stay tuned....

[BSmith23]

This is not exactly the answer you are looking for, but you could always add an extra pass or two to ease the chipload.  Yes, I understand it slows down the whole operation.  Just giving an alternate solution.

[cruzila]

You could make a dummy operation that just feeds one turn at whatever feedrate you are looking for. The Z depth would have to match but the top of the thread would be up about 032 incrementally.

[M Ham]

Thanks for all the great replies. I think I got my basic question answered as far as there being a function of Mastercam that would take care of this...NO.

I do one-off work, every piece unique, so tedious editing is usually not an option due to time constraints. Yes, using a 3 tooth Carmex and coding it as a single tooth so it does one continuous spiral per Carmex recommendations. I will conventional mill only because this is the most efficient method I have to get code out quickly. I prefer climbing for what I feel is better tool life and the chips fall away from the cutter as you progress.

Hoping to see something from Mastercam in the future as this is the only CAD/CAM software I have used that does not have a way to have an alternate feedrate for arc entries.

Thanks for the other interesting ideas on how to deal with this situation.

Regards, Mike

[gcode]

4 hours ago, M Ham said:

I will conventional mill only because this is the most efficient method I have to get code out quickly. I prefer climbing for what I feel is better tool life and the chips fall away from the cutter as you progress

Try the Carmes Hardcut line

They are left hand cutter (M04) 

To make a right hand thread you feed top down 

CDC is G42..  They work great in hard materials

I believe Harvey makes tools like this now as well