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
26
Post Thanks / Like
Likes (Given)
18
7

## 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
653
Post Thanks / Like
Likes (Given)
132
705
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
653
Post Thanks / Like
Likes (Given)
132
705
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
929
Post Thanks / Like
Likes (Given)
1094
573
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
653
Post Thanks / Like
Likes (Given)
132
705
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

9. Stainless
Join Date
Aug 2006
Location
Wisconsin
Posts
1,615
Post Thanks / Like
Likes (Given)
720
707
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.
I have often wondered this as well, I use Powermill and it can do outstanding things, it would think it would be simple to add that to the cam system. I usually split the toolpaths the best I can with steep and shallow areas for doing 3d work, having different speeds and feeds for each.

10. Cast Iron
Join Date
Mar 2017
Country
LATVIA
Posts
301
Post Thanks / Like
Likes (Given)
76
163
I'm saying this more from an electrical engineering POV - changing spindle speeds very often and rapidly puts a toll on the motor and its control, meaning - it takes/generates power to accelerate/decelerate quickly, power which needs to be drawn and dissipated, often machining center specs have nominal and max spindle power numbers listed, and those are calculated on some rough general estimates on how users use those machines, and if suddently some new milling strategy comes along that suddenly rises the "duty cycle" of a VMC spindle, problems may arise where there were none before

11. Aluminum
Join Date
Oct 2007
Country
UNITED STATES
State/Province
California
Posts
53
Post Thanks / Like
Likes (Given)
2
14

## Constant SFM with ball nose tools

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.
Hi G00:

While I haven't used this particular option, it does exist in the CAM program I use here, TopSolid.

12. Diamond
Join Date
Jan 2014
Country
UNITED STATES
State/Province
Washington
Posts
4,400
Post Thanks / Like
Likes (Given)
803
2366
Originally Posted by litlerob1
.....someone who is not talking out of their ass will chime in on the possibility of CSS on a Milling Operation......
I might be talking out my ass, but with the current method of speed control on a mill, a "faux" CSS scheme where S commands are added to the program as the effective tool diameter changes will not be surface friendly.

When a mill control executes the S command in a program, the command is sent to the PLC and program execution is halted waiting on an S command completion signal. The command is read by the PLC and processed through the ladder program. The result is sent to the spindle drive to change speed. Depending on how the ladder logic is written and some parameter settings that some popular controls use, the PLC may wait until the spindle drive confirms it has reached the new speed or some percentage of the commanded speed. Then the PLC sends the S command completion signal to the CNC which releases it to continue executing the program. How much time delay will occur depends on lots of factors. Could range from a few, to a few hundred milliseconds.

13. Titanium
Join Date
Nov 2014
Country
UNITED STATES
State/Province
Posts
2,706
Post Thanks / Like
Likes (Given)
3217
711
Originally Posted by Vancbiker
I might be talking out my ass, but with the current method of speed control on a mill, a "faux" CSS scheme where S commands are added to the program as the effective tool diameter changes will not be surface friendly.

When a mill control executes the S command in a program, the command is sent to the PLC and program execution is halted waiting on an S command completion signal. The command is read by the PLC and processed through the ladder program. The result is sent to the spindle drive to change speed. Depending on how the ladder logic is written and some parameter settings that some popular controls use, the PLC may wait until the spindle drive confirms it has reached the new speed or some percentage of the commanded speed. Then the PLC sends the S command completion signal to the CNC which releases it to continue executing the program. How much time delay will occur depends on lots of factors. Could range from a few, to a few hundred milliseconds.
This is only (on my part) a half arsed brain-fart...

On Okuma and MAZAK machines they have this "scheme" / method for chatter detection (with a microphone), on lathes there is this sinusoidal spindle speed 'Thing" (as most people know)... And for Mills picks another spindle speed that just moves off that "Mode" of vibration in-cut . I don't know if that "Pathway"/ channel can be hacked ?

I don't know if dynamically changing spindle speed beyond certain ranges will mess with available torque... + tool. Seems very machine specific for CAD CAM to implement (maybe). But kinda in the range that FalGrunt mentioned might be possible ? Barrel tools rather than ball-end mills for swarf milling type cuts.

I also wonder what it would sound like... [constant whining in the background or like a trip to the dental office (at lower RPM) , oooo, eeee wheeeee , oooooo, uuuuuh weee ooooo … like STOP ALREADY ! (combine that with x^3(cubed) acc and decc and jerk control...) ].

I agree it could mess with surface finish/ give unpredictable results. But interesting concept for 5 axis and different tool "Poise" angles vs. vector surface normal and tool engagement using a ball end mill vs SF/M.

__________________________________________________ __________________________________________________ _____

Intelligent Technology | Machining Navi | Okuma

14. Diamond
Join Date
Jan 2014
Country
UNITED STATES
State/Province
Washington
Posts
4,400
Post Thanks / Like
Likes (Given)
803
2366
Originally Posted by Vancbiker
......the current method of speed control on a mill......
This ^ was poorly phrased. Should have said mainstream or most common rather than current. As poinrted out by cameraman, there are some alternative speed control/adjustment technologies being used in select applications.

15. It would "seem" that it would be far easier (simpler?) to have the CAM software maintain a consistent engagement angle, and program the speed/feed for that? (if the geometry of the part allows that, of course).

Since SFPM and chip load are only valid at one infinitely small point "along the ball/sphere" (the cutter), wouldn't even a slight difference in amount of stock removed produce significantly different SFPM and chip load, vs. a cutter that is barely engaging the work (e.g. on a very fine finish pass)?

PM

16. Titanium
Join Date
Nov 2014
Country
UNITED STATES
State/Province
Posts
2,706
Post Thanks / Like
Likes (Given)
3217
711
Originally Posted by precisionmetal
It would "seem" that it would be far easier (simpler?) to have the CAM software maintain a consistent engagement angle, and program the speed/feed for that? (if the geometry of the part allows that, of course).

Since SFPM and chip load are only valid at one infinitely small point "along the ball/sphere" (the cutter), wouldn't even a slight difference in amount of stock removed produce significantly different SFPM and chip load, vs. a cutter that is barely engaging the work (e.g. on a very fine finish pass)?

PM
Not sure...

Circle Segment End Mills Increase Material Removal :

Modern Machine Shop

They're pushing circle segment end mills of different types but also stress the "CAM software, such as the more recent versions of HyperMill or Mastercam, is required to support and compute the geometries of the end mills for maximum performance."

The way things are grouped and organized in CAM how many tool paths are there where you use the flank(s)* of the tool and roll onto near the point and then back onto the main sides and (broader profile of tool ) in a continuous motion [And hence change spindle speed in cut ? ]. Swarf ---> tight radius ---> (back to) swarf (repeatedly + stepped … But that would be weird geometry to make sense ??? Unless you have a radially symmetric part (not saying anymore) + super rigid machine. ).

You can't have a vari-helix that gets tighter towards the narrower point as presumably the tool will choke ? Variable spindle speed dynamically and smoothly in cut.

So maybe someone is working on dynamic spindle speeds in-cut for new funky tools that only work with the most blinged out CAD CAM offerings ? And probably for very specific applications. [patent examiner's and notions of non-obviousness, don't really want speculate further as this is not my area and not want to give patent examiner's any fuel to ruin some one else's tea party/ bonfire / parade. "ordinary skill in the art" and "Non-obviousness.". ].

__________________________________________________ __

* flanks referring to principally the "sides" of the tool rather than the 'Flank" of a cutting edge as most of you will know "flank" of the tool as .

17. Stainless
Join Date
Mar 2011
Location
Huron
Posts
1,352
Post Thanks / Like
Likes (Given)
1895
845
I know that FeatureCAM has a routine to adjust the feed rate between two set points based on calculated chip load, I don't see why this isn't a thing. The program knows the surface normal to the cutter, it's simple math to get a new tool diameter, and ramp the spindle speed accordingly. I can't imagine it's too difficult to map the spindle accell/decell to a variable feed rate.

18. Titanium
Join Date
Nov 2014
Country
UNITED STATES
State/Province
Posts
2,706
Post Thanks / Like
Likes (Given)
3217
711
Originally Posted by Winterfalke
I know that FeatureCAM has a routine to adjust the feed rate between two set points based on calculated chip load, I don't see why this isn't a thing. The program knows the surface normal to the cutter, it's simple math to get a new tool diameter, and ramp the spindle speed accordingly. I can't imagine it's too difficult to map the spindle accell/decell to a variable feed rate.
In terms of mathematics, and programming (as in building stuff for the CAD/CAM side of things ) certainly doable, but as to rationale and practical application ? + different ways to spit out posted code where there may be more specific/ special codes to a specific machine beyond fairly standard G and M code ? (shrugging shoulders.).

For example is there a polynomial description for how a spindle should ramp up and down in cut ? I.e. map out it's curve in a way the machine would understand / perform smoothly ? Obviously some MTB's do this internally for their real-time chatter busting capability.

Would there be "rate of change" alarms that would be part of simulation code so one wouldn't tax a machine or ask for spindle accelations(sp) that are impossible etc. etc . ?

[Very speculative but possible ,... Practical ? ? ].

19. Originally Posted by primeholy
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?
You’ve been at it for 6-7 years OK & now the boss wants to optimize???

Finkl block (FX #2) is only slightly tougher than 4340 at the same strength level. You could search on that maybe.

Generally you do the whole approach time, productivity & cost and then find a happy place you can take to the bank. Finkl would prolly forward you some of their machining data & tooling used if you asked. The machinability chart below shows them running 363Bhn @ 200SFPM, .010IPR and 1/8”DOC for over an hour with .024” flank wear.

Good luck,
Matt