[Chris Duncan]

Doing a contour cut on a 1" thick piece of 6061 T6

short 1/2" end cutting HSS bit

1.0" DOC .020" WOC

GWizard says the most aggressive speed (rough cut) would be 135 IPM at 3900 RPM at .52 HP

So I turn it back to 80 IPM and try the cut. It's chattering and sounds like it's about to blow up and I can see the collet holder flexing, or something, it's going so fast it's hard to tell for sure

So I dial it back to 40 IPM and it makes a nice cut. This is the lowest speed/feed that GWizard gives for this cut.

Is anyone running their 770 at the max figures coming out of GWizard?

[RussMachine]

Not me.
I don't think GWizard actually takes the 1/2 Horsepower motor, and lack of rigidity into consideration.
I have a 770, and I frequently have problems with rigidity and chatter.
I've learned to slow my feeds down. WAAAYY Down.
The "recommended" settings mentioned (3500 RPM at 135 IPM) would give you a .035 feed per revolution. YIKES!!!
I'd bump the RPM up to 5000 (High Gear) and feed it at .002 per flute.

[Little_Chips]

You are not reading the info within GWizard correctly. The row labeled limits are machine limits not cut recipe limits. Look for the row labeled "Results" for the recipe. Under the setup tab select you can further refine the spindle power curve. You can get the HP Vs RPM from Tormach. In GWizard machine profile under Setup pick PCNC 770 then on the Spindle HP row click Adjust. This is where you can enter a refined power curve for the spindle.

I agree with RussMachine, in that GWizard is a little too agressive for my taste also.
You didn't say how many flutes you have so I guessed it was 2. I really like to use 3 flutes in 6061. I also like to use light rough and finish on the conservative - aggressive scale. I recommend you take a look at the manufacturers recommendation for chipload per tooth for the end mill. You can enter that in GWizard too.
I used .5", 2 flute, HHS, 1" DOC, .02" WOC, Selecting Agressive Rough on the rabbit, and I get 4272rpm @ 106.8ipm. I believe you would be using a rougher end mill for such a cut. At Light rough it is only 75ipm, and at Finish on the aggressiveness scale it is 46ipm. Also note the tips to the left of the aggressiveness scale. Climb milling is recommended. Conventional Vs climb milling can make a significant difference.

If you post the end mill specifics ie. Manufacturer and part number we may be able to provide more info. I like to start on the slower/less aggressive end of the spectrum then slowly speed things up. I break less end mills that way.

[menzzer37]

To make Gwizard more effective, use SFM input from the tool manufacturer. Gwizard is a great starting place for the Tormach under the Finish or Light Rough section. You really need to pay attention to stepover %, chip thinning, and DOC. I also have a Hurco and I use Gwizard for it with the tool mfg SFM. Cutting aluminum at 200% DOC, 6% stepover, 10,000 RPM @ 250 ipm with a 1/2" cutter. Ripping it

[wtopace]

Here's some cut recommendations from HSMAdvisor. I would recommend taking a larger WOC, as you are currently only at 4%, which is pretty small, even for HSM.

Data for your 4% cut:

Material: 6061-T6 Series Aluminum 95 HB
Tool: 0.500in 3FL Carbide None Solid End Mill
Speed: 1308.3 SFM/ 10000.0
Feed: 0.0037 in/tooth 0.0110 in/rev 110.00 in/min
Chip Thickness: 0.0014 in
Reference Chip load: 0.0043 in
Engagement: DOC1.00 in  WOC0.02 in
Effective Dia: 0.500 in
Cross Section: 0.08 x Dia.
Power: 0.66HP
MRR: 2.20 in^3
Torque: 0.35 ft-lb
Max Torque: 7.90 ft-lb
Cutting Force: 16.6 lb
Deflection: 0.0000 in
Max Deflection: 0.0012 in

Data for 10% WOC (where I usually start for HSM):

Material: 6061-T6 Series Aluminum 95 HB
Tool: 0.500in 3FL Carbide None Solid End Mill
Speed: 1308.3 SFM/ 10000.0
Feed: 0.0021 in/tooth 0.0063 in/rev 63.33 in/min
Chip Thickness: 0.0013 in
Reference Chip load: 0.0043 in
Engagement: DOC1.00 in  WOC0.05 in
Effective Dia: 0.500 in
Cross Section: 0.20 x Dia.
Power: 0.95HP
MRR: 3.17 in^3
Torque: 0.50 ft-lb
Max Torque: 7.90 ft-lb
Cutting Force: 24.0 lb
Deflection: 0.0000 in
Max Deflection: 0.0012 in

I would probably back the feed rate off in the overrides for the second cut since it's at 95% power rating of your machine and bump it up as it's cutting until you're happy.

Good Luck!

[Chris Duncan]

You are not reading the info within GWizard correctly. The row labeled limits are machine limits not cut recipe limits. Look for the row labeled "Results" for the recipe. ....

If you post the end mill specifics ie. Manufacturer and part number we may be able to provide more info. I like to start on the slower/less aggressive end of the spectrum then slowly speed things up. I break less end mills that way.

It's a 4 flute end mill. I moved the slow/fast slider back and forth and watched it change the "results" at the bottom. The numbers were just way higher than the numbers I had already been using without a calculator.

40 IPM and 4800 RPM made a nice cut. At 80 IPM it was flexing something in the upper Z unit you could watch the collet/bit jump over.

[Chris Duncan]

Gwizard is a great starting place for the Tormach under the Finish or Light Rough section.

That's what it's looking like. And an increase in RPM helped also.

[zero_divide]

It's a 4 flute end mill. I moved the slow/fast slider back and forth and watched it change the "results" at the bottom. The numbers were just way higher than the numbers I had already been using without a calculator.

40 IPM and 4800 RPM made a nice cut. At 80 IPM it was flexing something in the upper Z unit you could watch the collet/bit jump over.

If you are using gwiz make sure you are not using "HSM Speeds and Feeds" check box.
It will give you higher feedrate, more suitable for heavier machine. even when conditions do not really call for increase in either the feedrate or the spindle speed..

Either way I notice GWizard rely too much on rule of thumbs (ie. Half-light cut=x2 the feed)
rather than plain physics.

Well, your machining calculator is going to be only as good as the machinist who made it

[David Bord]

ouch...

[tmarks11]

I...Either way I notice GWizard rely too much on rule of thumbs (ie. Half-light cut=x2 the feed)
rather than plain physics.

unbiased review....



Although you do have a better resume than some of your competitors...

[zero_divide]

unbiased review....



Although you do have a better resume than some of your competitors...

If I think my calc (largely bulit on my machining experience. As it should.) is better, why can't mention it?

And Yep, I do machinin' for a living'

[Chris Duncan]

So the same parameters put into the free FSWizard gives 4970 RPM and 95 IPM

Since it's obvious the 770 isn't going to run at this rate, what do you suggest? Would you reduce by a certain factor?

40 IPM was working good. So multiply the calculated output by .42. But the RPM seems right so this is going to be difficult. Maybe just reduce the IPM and leave the RPM?

It would be nice if the calculators compensated for smaller machines. GWizard lets you select the machine you are using but obviously it's inaccurate with the 770.


Okay, I downloaded FSWizard Pro and it has the Tormach 770 selection, it still gives the 95 IPM


There is another factor here. The contour (perimeter) cut I'm doing has multiple angles and curves. It's really only at one angle on a large curve that the chattering really happens. I think it's analogous to when you are running a 1/4" angle die grinder in a large round hole and if you hold the die grinder at the same angle all the way around it will really chatter at certain places around the circle. Note also this is all climb milling.

But this factor is sort of immaterial since I'm not going to try to avoid a certain angle just to go faster.

[zero_divide]

So the same parameters put into the free FSWizard gives 4970 RPM and 95 IPM

Since it's obvious the 770 isn't going to run at this rate, what do you suggest? Would you reduce by a certain factor?

40 IPM was working good. So multiply the calculated output by .42. But the RPM seems right so this is going to be difficult. Maybe just reduce the IPM and leave the RPM?

It would be nice if the calculators compensated for smaller machines. GWizard lets you select the machine you are using but obviously it's inaccurate with the 770.


Okay, I downloaded FSWizard Pro and it has the Tormach 770 selection, it still gives the 95 IPM


There is another factor here. The contour (perimeter) cut I'm doing has multiple angles and curves. It's really only at one angle on a large curve that the chattering really happens. I think it's analogous to when you are running a 1/4" angle die grinder in a large round hole and if you hold the die grinder at the same angle all the way around it will really chatter at certain places around the circle. Note also this is all climb milling.

But this factor is sort of immaterial since I'm not going to try to avoid a certain angle just to go faster.

The version where you can set the machine is called HSMAdvisor.
It is obvious that there is a rigidity issue with 770.
What I am going from is the assumption that machine builder puts a motor with HorsePower suitable for the machine rigidity. In other words you should be able to utilize 100% of your horsepower and still get decent results.
Or at least that should not destroy your machine.

If you blindly apply some sort of reduction factor to your machine(you could reduce the available horsepower) you will needlessly go to too slow on many other opearations just for that one that causesd the issue.

IMO it is better to save the override in the Tool or a Cut in a tool database and next time you will get compensated results.

It is sometimes the case even with bigger machines and having all sorts of little adjustments is normal in the trade.

[SCzEngrgGroup]

It would be nice if the calculators compensated for smaller machines. GWizard lets you select the machine you are using but obviously it's inaccurate with the 770.

No calculator is going to give you perfect, optimal numbers every time - there are simply too many variables that are basically unknowable, and no two machines are exactly alike. Even the specific tool you choose has a major impact. I've found I can buy two seemingly identical endmills from different manufacturers, and one will work beautifully, while the other will chatter like crazy even with the feed backed off 50%. You need to use the calculator as a tool to tell you what's possible, then see how close you can get with your machine, and your tooling. If you can't even get close, then either there is a problem with a) the machine (low rigidity, low power, backlash, etc.), b) the setup (poor clamping, a non-rigid workpiece, etc.), c) poor tooling (low stiffness, resonance that lies at or near a machine resonant node of the machine), or d) just a bad tool. Try different tools, and when you find ones that work well on YOUR machine stick with them. Buying random endmills will never give you an ideal result. Years ago, I spent a lot of time and money buying different endmills and testing them extensively. I found the ones that work best on my machine, and the kind of work I do, and I never buy anything else. Spend the small amount of money for HSMAdvisor. It is excellent when used properly. I tried GQizard many time, and found it sadly lacking in many respects, not the least being it would (seemingly) randomly give completely garbage results. This whole exercise was time-consuming, but resulted in being able to get my parts done in 1/2 to 1/3 the time was before.

Also, for a small machine like the 770 cutting 6061, don't waste money on Carbide tooling, except for smaller endmills (1/4" and below). Over 1/4", HSS will work just as well, for a lot less money. Below 1/4" the added stiffness of carbide is worthwhile. Above that, you don't have enough power, or rigidity, to get much, if any, benefit from carbide. For steel and other harder materials, carbide is appropriate. I do the bulk of my 6061 work with 1/2" HSS 2-flute endmills at well over 100 IPM, and I'm limited by spindle power. Without a higher RPM, more powerful spindle, I'd gain nothing by using carbide.

Regards,
Ray L.

[AUSTINMACHINING]

I would use a high helix 3 flute end mill. The yg-1 alupower is awesome in aluminum. For roughing I run the 1/2" end mill 100 IPM, .05" step over .6" deep, 6000 rpm per HSM ADVISOR. Works great.finish at full depth of cut, 3% of the end mill diameter 35IPM for a mirror type finish.

[Chris Duncan]

I agree with you on the carbide and aluminum. With the lack of rigidity and the chatter, they end up chipping anyway.

So what machine are you running with 1/2" HSS 2-flute endmills at well over 100 IPM

Do you recommend 2 flute over 4 flute? What is the max RPM you run?

The only problem I have with HSS endmills is they don't come with corner radius, or at least I haven't found them.

Here are the areas on the part where it is chattering, it's like on a certain area of an arc. It's even got a really light chatter at 40 IPM in these areas which shows up as slight surface roughness.

The other parts of the perimeter were actually sort of okay at 80 IPM although the machine seemed at it's limit.

Attachment 302634

[Chris Duncan]

I would use a high helix 3 flute end mill. The yg-1 alupower is awesome in aluminum. For roughing I run the 1/2" end mill 100 IPM, .05" step over .6" deep, 6000 rpm per HSM ADVISOR. Works great.finish at full depth of cut, 3% of the end mill diameter 35IPM for a mirror type finish.

What machine is this?

[RoketRdr]

Well, your machining calculator is going to be only as good as the machinist who made it

It works perfectly fine. And the experienced machinist who made it did an excellent job. Contrary to popular belief a calculator cant correct user error.

[AUSTINMACHINING]

What machine is this?

Novakon torus pro.

Sent from my SM-G900T using Tapatalk

[Chris Duncan]

Contrary to popular belief a calculator cant correct user error.

Dang it. Now I'm in trouble.