Calculating surface feet ball nose tooling

# Thread: Calculating surface feet ball nose tooling

1. Plastic
Join Date
Sep 2016
Country
UNITED STATES
State/Province
Tennessee
Posts
7
Post Thanks / Like
Likes (Given)
3
0

## Calculating surface feet ball nose tooling

Hello. I am a programmer at a forge plant. Our dies are made out of Finkel grade 2(fx2) material. We have been using the same F.R. and rpms for 6-7 years now. My boss is wanting me to optimize our cutting parameters. Do you guys/gals have any suggestions on calculating surface feet and recommended doc/stepover for die steels? Any good resources?

2. Hot Rolled
Join Date
Feb 2013
Country
UNITED STATES
State/Province
Idaho
Posts
530
Post Thanks / Like
Likes (Given)
107
592
Basically your surface feet per minute decreases to zero at the cutting tip. In other words, use the standard formula RPM/3.82 X Cutter Diameter, but instead of the actual cutter diameter, you can approximate the diameter at the actual point of contact of the tool. If you are using the absolute tip, the diameter approaches zero and that is why you will see rubbing and tip degradation. There are some ways around this. First, if you have the opportunity, approach the surface from the bottom rather than the top. This will move the point of contact out from the tip, increasing the SFM. Second, most shops that are doing a bunch of surfacing, use tools other than traditional ball endmills. For instance, any sort of bull endmill. There is also a growing trend to use barrel tools for steep surface and large radius lense tools for shallow surface. These have a twofold advantage of increasing the SFM and increasing the effective radius to produce a finer surface finish with a larger stepover. Mastercam (and I'm sure others) has done a good job of using these new tools in their multiaxis surfacing routines.

Lastly, when the opportunity presents itself, I like to rotate the part being machined in the A axis by a couple of degrees. This prevents me from machining with the actual tip of the cutter, and pushes the point of contact out towards the major diameter increasing the SFM even on low angle surface. This is free, but only applicable in 4 and 5 axis mill work. On my 3 Axis machines, I tend to use bull endmills. As far as actual feeds and speeds, I can't help you with that material, and stepover is very dependent on the type of toolpath you are running in the cam system (scallop, waterline, parallel....)

3. Hot Rolled
Join Date
Feb 2013
Country
UNITED STATES
State/Province
Idaho
Posts
530
Post Thanks / Like
Likes (Given)
107
592
Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing. Very similar to how a lathe alters the RPM while facing. It wouldn't be a simple calculation, but it could be done. Especially for applications where you are surfacing hard materials (low SFM) with a high potential RPM spindle... shower thoughts.

4. Hot Rolled
Join Date
May 2017
Country
UNITED STATES
State/Province
Minnesota
Posts
658
Post Thanks / Like
Likes (Given)
544
342
Originally Posted by G00 Proto
Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing.
Probably because most surface finishing routines are not stock aware. Might not hurt to send a feature request to Vericut for their toolpath optimization suite; if anyone can do it they can.

5. Originally Posted by G00 Proto
Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing. Very similar to how a lathe alters the RPM while facing. It wouldn't be a simple calculation, but it could be done. Especially for applications where you are surfacing hard materials (low SFM) with a high potential RPM spindle... shower thoughts.
It's not a question for the CAM developers. It's motion control, ladder logic, spindle mechanics. There's a lot more to it than just a code.

R

6. Hot Rolled
Join Date
Feb 2013
Country
UNITED STATES
State/Province
Idaho
Posts
530
Post Thanks / Like
Likes (Given)
107
592
Originally Posted by litlerob1
It's not a question for the CAM developers. It's motion control, ladder logic, spindle mechanics. There's a lot more to it than just a code.

R
I'm not sure that I agree (not trying to be argumentative since this is largely an academic question at this point). I think that the spindle speed optimization could be controlled at the cam level based on the SFM at the calculated effective radius of a ball nose endmill. The question that you nailed is could the change in spindle speed keep up with the programmed change in spindle speed. It would be pretty easy on a waterline toolpath, but very difficult on a parallel toolpath where the z (and effective cutter diameter) is constantly changing. I think that it is something that could be done on certain toolpaths. Like I said, "shower thoughts" I gotta admit, I am always amazed by how my turning center alters the RPM based on the effective diameter of the stock, pretty cool if it could do the same thing on mill toolpaths. Then again, I'm pretty simple and a lot of things amaze me... probably as a result of sniffing burnt coolant for too many years>

7. I guess you might be right, someone who is not talking out of their ass will chime in on the possibility of CSS on a Milling Operation.

Theoretically you could do it manually in the program, by doing all the maths and changing the RPM at every elevation change. Line for line, it wouldn't be a huge leap for a CAM developer to add that into the Macro/Variable in the Post Processor. But it would be a huge amount of Data. Even doing it as per the Tool diamter wouldn't be too hard, you wouldn't need to Map the Surface for Elevation. The Toolpath itself would need to be off a Surface or a Net. So the software knew what diameter it would be using. Shit maybe.

R

8. If the magical gremlins know a .02cr tool is using the top of the radius at the top of generating a 1/2” radius and the bottom of the radius at the bottom, I don’t know why the couldn’t say, 12k rpm at the bottom and 10k at the top?

Disclaimer: those are all completely random numbers