Keyseat Cutter - To Interpolate or Not To Interpolate?

I've attached the blueprint of the part to be made, photos of the actual part, the drawing of the carbide tool (it’s custom) and actual photos of the tool that I'll use to cut the feature in question.
I'm making this part on a Citizen L32 (Swiss machine). This operation is taking place on the main spindle, in guide bushing mode. The tool is running in an ER20 live tool. The material is 4140.
The tool is 1.000” diameter (.500” radius) and the blueprint calls for a .500” radius so initially I tried plunging the tool to depth. The photos of the part show the results of this, it chattered. I’ve just discovered the tool doesn’t have the proper relief behind the cutting edge (see photo) and is rubbing, causing a heavy burr and excessive tool pressure, which I’d say is contributing to the chatter.
Considering cycle time, I thought plunging would be the preferred method, agreed? Now I’m beginning to think that I should try and interpolate this feature, any thoughts?
Any help/insight will be greatly appreciated!

If I'm reading that print correctly it looks like a Acme thread milling cutter would work fine. That would be in the 28° +4-0 on the angle.

I would interpolate it and make passes starting at about 0.25 DOC and reduce on each subsequent pass until the proper depth is reached.

i would think that by using a smaller dia. cutter and generate the form would be better
you might also try and go with 5 flutes instead of ten this could allow better secondary relief to eliminate the rubbing
how stable is the er20 spindle that you are using ? just curious do having just started working on an l32x. Is this a half speed spindle for better torque?

Quote:

---

Originally Posted by Jim Dawson

If I'm reading that print correctly it looks like a Acme thread milling cutter would work fine. That would be in the 28° +4-0 on the angle.

I would interpolate it and make passes starting at about 0.25 DOC and reduce on each subsequent pass until the proper depth is reached.

---

"Acme thread milling cutter" would something like this (https://www.mscdirect.com/product/details/44076826) work? The angle will suffice but how about the .08 +.02/-.00 dimension and the .175 +.02/-.000 dimension? The tool is listed as 6
TPI, I was thinking that the TPI with this tool isn't a given (it could be changed via the program), the only given is the angle of the tool, is this correct?

Quote:

---

Originally Posted by rcs60

i would think that by using a smaller dia. cutter and generate the form would be better
you might also try and go with 5 flutes instead of ten this could allow better secondary relief to eliminate the rubbing
how stable is the er20 spindle that you are using ? just curious do having just started working on an l32x. Is this a half speed spindle for better torque?

---

I agree with the smaller diameter cutter idea. We don't have CAD/CAM software in the shop and I'm not exactly sure how to generate the tool path since it's not a complete/full radius, any suggestions.
Do you have any recommendations for a tool manufacturer that would make this custom tool?
The ER20 is relatively stable, of course I'd prefer something more robust but that's the largest that the machine can handle. The ratio of the ER20 is 1:1.

Thank you for the reply.

It looks like a 4 TPI tool would fall in the specs. You would cut 0.184 deep. I don't see a depth spec on the print but maybe I missed it.

https://www.amesweb.info/Screws/Acme...imensions.aspx

...

Quote:

---

Originally Posted by Jim Dawson

It looks like a 4 TPI tool would fall in the specs. You would cut 0.184 deep. I don't see a depth spec on the print but maybe I missed it.

https://www.amesweb.info/Screws/Acme...imensions.aspx

---

Thank you for the response and for sharing the calculator. My apologies for the delayed response. The .09" (nominal) dimension on the print will be achieved as well as the angle, but I'm not sure about the .185"(nominal) dimension?
The depth isn't called out, but the distance from the cutting edge of the tool to the shank of the tool has to be roughly .308" minimum. I agree with the .184" deep, but where the radius breaks through into the tapered section at the highest point (zenith) to the OD(.834" section) is the .308"
Again, thank you for your time Jim.

Quote:

---

Originally Posted by NiCu2829

I've attached the blueprint of the part to be made, photos of the actual part, the drawing of the carbide tool (it’s custom) and actual photos of the tool that I'll use to cut the feature in question.
I'm making this part on a Citizen L32 (Swiss machine). This operation is taking place on the main spindle, in guide bushing mode. The tool is running in an ER20 live tool. The material is 4140.
The tool is 1.000” diameter (.500” radius) and the blueprint calls for a .500” radius so initially I tried plunging the tool to depth. The photos of the part show the results of this, it chattered. I’ve just discovered the tool doesn’t have the proper relief behind the cutting edge (see photo) and is rubbing, causing a heavy burr and excessive tool pressure, which I’d say is contributing to the chatter.
Considering cycle time, I thought plunging would be the preferred method, agreed? Now I’m beginning to think that I should try and interpolate this feature, any thoughts?
Any help/insight will be greatly appreciated!

---

I've attached the blueprint of the part to be made and my code to machine the 5 slots in the OD. My goal is to have a program that regardless of the tool diameter, programmed radius or # of passes/DOC can be changed with relative ease. I'd like to make #527 passes where each pass is #528/#527 deep (the actual DOC is [#528/#527]/2 because the Y axis is diametrical).
I've never used variables to this extent so I'm hoping y'all will look it over and critique my code.


In the program I accounted for the key cutter tool radius when I programmed the tool path, so the R value on the offset screen=0.


I'm cutting on the minus(-) side of Y0.


Thanks in advance!