HSM Speed and feed check please

Volitan · Jan 19, 2018

I've got a 3/16" hotmill, 5/8" loc, cutting .610 deep in 1018 steel.
What kind of chipload and stepover would be good to start? My usual 12% stepover starting point seems a bit much for this tool and I don't have HSM Advisor on the work PC yet.

Thanks

dodgin · Jan 19, 2018

I'd think that about an 8% stepover with about .0015 FPT chipload would be a start that wouldn't result in a snapped off endmill.

B-Mathews · Jan 19, 2018

Per FS Wizard

662 F/min
FZ 0.001

Doc 0.610
Woc 0.010

OR

DOC 0.318
WOC 0.020

Volitan · Jan 19, 2018

Thank you!!

Matt@RFR · Jan 19, 2018

I'd be more like 5-6% stepover and .002 - .0023 IPT. This assumes you have the RPM to be in the 600+ SFM range. Get those chips cleared or you'll be breaking tools.

Atomkinder · Jan 19, 2018

HSMAdvisor is giving me 6.9% rDOC and .00244 chipload, which translates to 12k RPM @ 117.31IPM for a Haas VF-SS spindle.

Here's the info box text:

Material: 1018 (126 HB)
Tool: 0.188in 4FL Carbide AlTiN Solid End Mill
Speed: 588.7 SFM/ 12000.0RPM
Feed: 0.0024 in/tooth 0.0098 in/rev 117.31 in/min
Chip Thickness: 0.0012 in
Reference Chip load: 0.0012 in
Engagement: DOC=0.61 in WOC=0.01 in
Effective Dia: 0.188 in
Cross Section: 0.22 x Dia.
Power: 0.5HP
MRR: 0.93 in³
Torque: 0.22 ft-lb
Max Torque: 0.42 ft-lb
Cutting Force: 27.7 lb
Deflection: 0.0015 in
Max Deflection: 0.00500 in

B-Mathews · Jan 19, 2018

I find it annoying how far apart the FS Wizard app and HSM adviser can be off in speeds and feeds.There both for the same maker but use different algorithms. Both seem to cut well but the HSM is much more aggressive. I was not in the shop or I would have given him the HSM info.

Thanks Atom.

Volitan · Jan 19, 2018

I'm cutting .240 wide slots in 5/16" thick pieces .610 deep, using the "peel mill" feature in Mastercam which is pretty nice.

This worked good. Feel bad for the machine though. 2,000 pieces, we may end up stepping down or something else.

zero_divide · Jan 19, 2018

B-Mathews said:
I find it annoying how far apart the FS Wizard app and HSM adviser can be off in speeds and feeds.There both for the same maker but use different algorithms. Both seem to cut well but the HSM is much more aggressive. I was not in the shop or I would have given him the HSM info.

Thanks Atom.

I find it annoying too!
Old FSWizard uses different outdated math.
New one, which is not yet available on Play or iTtunes (but available here: FSWizard Speed and Feed Calculator) gives much closer results.

But still, it may never match HSMAdvisor in complexity just because it is near impossible to fit all that stuff inside a small mobile app.

So some discrepancy at edge cases will still remain.

B-Mathews · Jan 19, 2018

zero_divide said:
I find it annoying too!
Old FSWizard uses different outdated math.
New one, which is not yet available on Play or iTtunes (but available here: FSWizard Speed and Feed Calculator) gives much closer results.

But still, it may never match HSMAdvisor in complexity just because it is near impossible to fit all that stuff inside a small mobile app.

So some discrepancy at edge cases will still remain.

Thanka Edger. I thought at one point you had bagged the App side of things and where just gonna go with the HSM Adviser. Glad to hear there is the new one coming. That said I love what you have done. It has really helped me optimize my parts.

Speedie · Jan 19, 2018

.005 deflection..is that tool deflection?

zero_divide · Jan 19, 2018

Speedie said:
.005 deflection..is that tool deflection?

Nah. Tool deflection is 0.0015

0.005 is the maximum safe value. Can handle even more. But in case of small tools deflection will add to subsequent width of cut that will eventually break the tool.

Volitan · Jan 22, 2018

I ended p backing off on the feedrate and upping the stepover a little, and got the demo version of HSMAdvisor installed. I got the OK to buy it after the time is up which is nice.

Was just playing around with the C-Hook in Mastercam 2018, very nice! They should pay you to just include it with every seat.

Material: 1018 (126 HB)
Tool: 0.188in 4FL Carbide TiAlN Solid End Mill
Speed: 343.4 SFM/ 7000.0RPM
Feed: 0.0018 in/tooth 0.0071 in/rev 50.00 in/min
Chip Thickness: 0.0010 in
Reference Chip load: 0.0012 in
Engagement: DOC=0.61 in WOC=0.02 in
Effective Dia: 0.188 in
Cross Section: 0.26 x Dia.
Power: 0.2HP
MRR: 0.46 in³
Torque: 0.18 ft-lb
Max Torque: 0.42 ft-lb
Cutting Force: 23.4 lb
Deflection: 0.0013 in
Max Deflection: 0.00533 in
Comment: 3/16" 4F Regular, Square, TiAlN coated Solid Carbide Endmill
Operation Comment:
Additional Operation Info:

zero_divide · Jan 22, 2018

Volitan said:
I ended p backing off on the feedrate and upping the stepover a little, and got the demo version of HSMAdvisor installed. I got the OK to buy it after the time is up which is nice.

Was just playing around with the C-Hook in Mastercam 2018, very nice! They should pay you to just include it with every seat.

Yeah we were discussing that but it kind of died off. Perhaps they will change their mind once i release the public SDK

I am glad my software could be of help!

Search

Largest Manufacturing Technology Community on the Web

Search

HSM Speed and feed check please

Volitan

Hot Rolled

dodgin

Hot Rolled

B-Mathews

Hot Rolled

Volitan

Hot Rolled

Matt@RFR

Titanium

Atomkinder

Titanium

B-Mathews

Hot Rolled

Volitan

Hot Rolled

zero_divide

Stainless

B-Mathews

Hot Rolled

Speedie

Stainless

zero_divide

Stainless

Volitan

Hot Rolled

zero_divide

Stainless

Similar threads