MFG speeds & feeds recommendations vs G wizard/HSM adviser ( I am a newbie)

Hello everyone,



I am on day 3 of trying to pick the right feeds & speeds for my first cnc part on a Tormach 1100. I am getting 3 different inputs from my sources. This is driving me nuts as it is the only part I am not confident on. This is all on a 3d adaptive tool path



I am cutting 6061 alu. with a HSS uncoated 2 flute 3/8 end mill which is pretty long. Below are the details of the end mill:

Cutting dia : .375

Flute length: 2.495

Overall length: 4.25

Body length: 3.1

Shaft dia: .375



I contacted the MFG for their recommendation and got it https://heritagecutter.com/BrubakerWeldon/PublicStore/Downloads/Brubaker M7-M42-PM End Mill-No...



CALCULATIONS FOR SPEED CALCULATIONS FOR FEED
RPM = (3.82 x SFM) / DIA. IPM = # of FLUTES x FPT x RPM
SFM = (RPM x DIA.) / 3.82 FPT = IPM / (RPM x # of FLUTES)



The Tormach 1100 does 5100 RPM and I was told to keep the RPMS up near max for alu. which means:



First I calculated the SFM:

(5100x.375) / 3.82 = 500.654 THIS IS SFM VALUE



Then, I calculated IPM

2 x .0041 x 5100 = 41.82 ( 2 flutes, what the mfg says FPT is, RPM)



So unless I am mistaken in Cam, my values should be:



5100 RPM

500.654 SFM

41.82 for lead in/out. Fusion recommends .00385 feed per tooth and when I enter the .0041 feed per tooth value the cutting feed rate goes up to 41.82 as my math suggests it should. I was comfortable with this, until I tried out G wizard and HSM adviser which recommended wildly varying values.



HSM says:



.4 DOC (maximum step down) .15 WOC (step over)



5120 RPM

1.37 in/min feed

502 in/min speed

.00013 chip load

.81 plunge feed



It also says .04HP used, .04 lb/ft of tq used, and tool deflection is in the red at .0020 deflection or 19.8%. I was told to keep deflection under .001?



G wizard says done at 50% between conservative and aggressive:

4504 RPM

14.627 IPM Feed

7.3 Plunge speed

442 SFM

.0016 chip load

.003 tool deflection? it has the % at 334%!!!



Please help me guys, I have googled, read and exhausted all my friends ears with this. I get very generic responses to the effect of " I just feel it out" that do not inspire confidence. What am I overlooking? Am I using these calculators wrong?

I get my feeds and speeds from some software that I bought in the late 80's. Recommended feeds and speeds are just a starting point, many times you can go way faster and other times you must slow down. Considering you have a Tormach you probably will have to go quite slower than recommended speeds and feeds due to a lack of horse power and rigidity. This is a forum of mostly professionals in production environments, so there probably aren't many users of Tormachs here. Where are you at in Virginia? I am about 45 miles NW of Richmond. Sourcing supplies and outside services seem to be a PITA in this state and I have been here 8 years.

Not to throw you another curve ball, but if your 6061 is Chinese it can easily gum up end mills and you will have to not cut it as aggressively as a good domestic or European brand.

You know, I never considered the MFG assumes the end user will have an actual VMC. You think I should do a run with the Gwizards speeds and feeds THEN adjust? Yes, the Tormach is under powered but a Vf2 or a Mini mill 2 is coming in the winter if I can get the hang of this.

I'm dead in the middle of RVA. I have basically had to narrow down my new machine purchase to HAAS because they are the only ones who I have seen have a dealer network or servicing in the area. I really wanted a Brother, Hurco, etc but if it goes down I know i'd be left to my own devices. Has that been your experience as well?

Dualkit said:

Not to throw you another curve ball, but if your 6061 is Chinese it can easily gum up end mills and you will have to not cut it as aggressively as a good domestic or European brand.

Click to expand...

It is from Mcmaster Carr, I figured it'd be a safe choice. a 3.5 x 3.5 square 12" long was 82.00 before shipping. Any experience?

Since you have Tormach I would go with the G wizard values. It will be fine.

Pretty slow compared to how I might run it on a bigger machine but the lack of aggressiveness is good for an amateur setup/machine.

First, that tool is really long and skinny, it's going to cause issues, exacerbated by a tormach. Any manufacture chart is likely not expecting that fragile of a tool.

"RPM near max" is too general for my taste, especially with an uncoated HSS cutter. They don't know your machine. I'd go to another source which is based off the material and the cutter diameter for SFPM, but 4000-5000 RPM probably fine with coolant. With aluminum you'll need to worry about BUE if you're not using coolant. If that's the case I'd start with half that RPM. This will be less likely to weld the edge and you'll be able to keep a much closer eye on things, i.e. things won't go south as fast.

0.004 IPT is aggressive for a 3/8" cutter, especially at that flute length. Some cutter manufactures will give you a max DOC and WOC for their recommended feed for a given diameter tool (like 2D DOC and 0.25D WOC) and guidance as to what to do for larger DOC. Usually it involves feeding slower and less WOC. I definitely wouldn't start more than 2x cutter diameter for DOC or 0.75", and personally with that length I'd go no more the 0.020" WOC to start, it's a really long skinny cutter and that's likely causing your high deflection numbers. 0.150" WOC seems very aggressive.

The HSM feed is too low, almost rubbing. It may be being influenced by deflection, I've never used HSM or G-wizard. The G wizard feed is much better. Again both deflection numbers likely being influenced by the large WOC and very skinny tool.

BWS JAZE said:

The Tormach 1100 does 5100 RPM and I was told to keep the RPMS up near max for alu. which means:

Click to expand...

Sure, most of the time you'll be near the max, but longer cuts you'll want to drop the RPM, like full LOC on your end mill or chatter will ensue. I use HSM advisor and am very fond of it, however, it will tell me to go way too fast some times. In your case, I'd start slow if you are in doubt. Easier to bump it up then realize you went too fast and have a trashed part, broken cutter.

I'd pick up a 3 flute carbide end mill and ditch the HSS. Maritool has lots of flavors.

JCByrd24 said:

First, that tool is really long and skinny, it's going to cause issues, exacerbated by a tormach. Any manufacture chart is likely not expecting that fragile of a tool.

"RPM near max" is too general for my taste, especially with an uncoated HSS cutter. They don't know your machine. I'd go to another source which is based off the material and the cutter diameter for SFPM, but 4000-5000 RPM probably fine with coolant. With aluminum you'll need to worry about BUE if you're not using coolant. If that's the case I'd start with half that RPM. This will be less likely to weld the edge and you'll be able to keep a much closer eye on things, i.e. things won't go south as fast.

0.004 IPT is aggressive for a 3/8" cutter, especially at that flute length. Some cutter manufactures will give you a max DOC and WOC for their recommended feed for a given diameter tool (like 2D DOC and 0.25D WOC) and guidance as to what to do for larger DOC. Usually it involves feeding slower and less WOC. I definitely wouldn't start more than 2x cutter diameter for DOC or 0.75", and personally with that length I'd go no more the 0.020" WOC to start, it's a really long skinny cutter and that's likely causing your high deflection numbers. 0.150" WOC seems very aggressive.

The HSM feed is too low, almost rubbing. It may be being influenced by deflection, I've never used HSM or G-wizard. The G wizard feed is much better. Again both deflection numbers likely being influenced by the large WOC and very skinny tool.

Click to expand...

Thank you for that, it helps tremendously. I guess I should reconsider my choice of end mill for this part in the future. It is adding up to me as that this end mill is pretty much a finishing end mill for peripheral milling? and not for roughing. Can't imagine what that end mill's real world application would be.

CosmosK said:

Sure, most of the time you'll be near the max, but longer cuts you'll want to drop the RPM, like full LOC on your end mill or chatter will ensue. I use HSM advisor and am very fond of it, however, it will tell me to go way too fast some times. In your case, I'd start slow if you are in doubt. Easier to bump it up then realize you went too fast and have a trashed part, broken cutter.

I'd pick up a 3 flute carbide end mill and ditch the HSS. Maritool has lots of flavors.

Click to expand...

Thank you for the response. Yes, I think the end mill is just not a good fit for the operation type. I imagine something like a shear hog would be ideal for this. I am a newbie at CNC but a vet in fabrication and I know the tool is only as good as the guy using it so a specialized tool like that seemed out of my capacity. I can see why people call this job/hobby a rabbit hole at the bottom of a money pit.

BWS JAZE said:

Hello everyone,
I am on day 3 of trying to pick the right feeds & speeds for my first cnc part on a Tormach 1100. I am getting 3 different inputs from my sources. This is driving me nuts as it is the only part I am not confident on. This is all on a 3d adaptive tool path

I am cutting 6061 alu. with a HSS uncoated 2 flute 3/8 end mill which is pretty long. Below are the details of the end mill:

Cutting dia : .375
Flute length: 2.495
Overall length: 4.25
Body length: 3.1
Shaft dia: .375

HSM says:

.4 DOC (maximum step down) .15 WOC (step over)
5120 RPM
1.37 in/min feed
502 in/min speed
.00013 chip load
.81 plunge feed
It also says .04HP used, .04 lb/ft of tq used, and tool deflection is in the red at .0020 deflection or 19.8%. I was told to keep deflection under .001?

Please help me guys, I have googled, read and exhausted all my friends ears with this. I get very generic responses to the effect of " I just feel it out" that do not inspire confidence. What am I overlooking? Am I using these calculators wrong?

Click to expand...

Right here HSMAdvisor is telling you are going to have trouble:



By default HSMAdvisor is limiting your deflection to 100%
It is still surviveable and you will get RPM: 5120 feed 12ipm

But you chose to limit the deflection to 0.001" and HSMAdvisor obviously has no other choise but to reduce your feedrate to rubbing.

To keep the feed rate sendible you need to reduce one(or more) of the following:
* Tool Stickout - it is VERY large for HSS tool
* WOC and/or DOC - 0.150 x 0.40 is waay too heavy.

There is no way on earth you are going to keep deflection under 0.001" with this kind of tool. You need to chuck it shorter OR reduce the WOC/DOC way down.

Is this roughing or finishing?
If i was stuck with this tool configuration i would do something like this:


And then still you would have to play with DOC and RPM to make sure it does not chatter like crazy.

Regards.

EDIT: i just noticed that you have very large flute length too, so please DO NOT use the calculations as is, but enter your actula flute lenght as the values will be drasticly different!!!:

BWS JAZE said:

It is from Mcmaster Carr, I figured it'd be a safe choice. a 3.5 x 3.5 square 12" long was 82.00 before shipping. Any experience?

Click to expand...

McMaster Carr is pretty good with selling quality products, it is likely either domestic or a decent European brand, not Chinese trash.

OP, there's some really serious talent replying here. (not me)
Shorter is better for end mills - use the shortest one you can. Often it's best to even use multiple, starting with shorter if you simply must use longer to finish. I've never run a Tormach. I've seen people make some nice parts on them - but they are not known for rigidity. Help your mill out by keeping every end mill as short as you can. Experience can be a dear teacher. Using a smaller machine might require you to become creative in how you approach projects. Good luck!

Do you need that long of a flute length for your part? If not, then I highly recommend dropping your length of cut, else broken endmills are sure to result.
If you must cut that deep, a larger diameter tool, or a solid carbide endmill with a stub flute and reduced shank might get you there with shorter stepdowns and light cuts. You're somewhere around 6xD. Deeper than about 2xD I start backing things down usually, and deeper than 4xD I usually look for alternate options or at least take very special care in setup and programming to maximize my chances of success. Maybe variable flute tooling to reduce vibration, for example.