HSMAdvisor vs G-Wizard vs Free calc?!

[zero_divide]

0.25 DOC and 0.07 WOC..HSS


Ray, I posted from my phone. Only posted part of my reply, sorry.

HSS .25 DOC .075 WOC 3 flute 3/8's cutter 4000 rpm 392 sfm and 48IPM is what Inventor HSM and HSMadvisor is saying.

If roughing:


But that is a rather light cut. You probably will not even have to use coolant.

[AUSTINMACHINING]

I set the desired parameters and start,at 50% and bump up the feed and monitor spindle speed/load. Also, the is a big difference in tool type/geometry. Typically 3 cu in/min per hp in aluminum. I have a 1/2" zrn serrated rougher from maritool that i can push to 4 cu in/min.These little machines run out of power quick, and it's a fine line between max MRR and stalling the spindle.

[C*H*U*D]

@

Wish I can find a good starting feed/speed for the 770.

Something like this?

[narrobb]

Thanks. I actually watched that recently. Very helpful.

Like everything else, if a newbie followed same data like a pro, it won't have the same result! There are too many other variables at play and you can't fix all. I am convinced it will come with experience and experimentation.

Today, the calculator showed me that I can indeed slot through a 1.2" 6061-T6 using 3800 RPM 8 IPM, with 0.5" 2F HSS, and using 0.6" DOC and of course 1/2" WOC as it's the Dia. This is using Tormach 770 as selected machine but dialed down. Didn't work.

So instead as a learning operation, I did it in multi-pass with each pass different RPM and Feeds. DOC varied between 0.05" and 0.2". This is all good, it's all part of the learning curve and every newbie got to go through testing.

Something like this?

[zero_divide]

Thanks. I actually watched that recently. Very helpful.

Like everything else, if a newbie followed same data like a pro, it won't have the same result! There are too many other variables at play and you can't fix all. I am convinced it will come with experience and experimentation.

Today, the calculator showed me that I can indeed slot through a 1.2" 6061-T6 using 3800 RPM 8 IPM, with 0.5" 2F HSS, and using 0.6" DOC and of course 1/2" WOC as it's the Dia. This is using Tormach 770 as selected machine but dialed down. Didn't work.

So instead as a learning operation, I did it in multi-pass with each pass different RPM and Feeds. DOC varied between 0.05" and 0.2". This is all good, it's all part of the learning curve and every newbie got to go through testing.

It probably stalled the spindle.

Power calculations only make sense when feedrate is close to ideal values.

When you have to go so deep, HSMAdvisor would reduce your feedrate considerably which would lead to more friction and spindle stalling.

[joshetect]

1/2" is on the larger side for these machines. If you are trying stuff out, try a smaller endmill. Going with a smaller endmill then the slot needs to be will also give you a nicer finish on both walls.

[Advil]

When I run the numbers on your slotting operation with a 1/2" end mill (that's a big frickin end mill for a 770 especially for a slotting op) I get this cutting data:

Material: 6061-T6 Series Aluminum 95 HB
Tool: 0.500in 2FL HSS None Solid End Mill
Speed: 480.0 SFM/ 3668.8RPM
Feed: 0.0032 in/tooth 0.0064 in/rev 23.48 in/min
Chip Thickness: 0.0032 in
Reference Chip load: 0.0032 in
Engagement: DOC=0.17 in WOC=0.50 in
Effective Dia: 0.500 in
Cross Section: 0.33 x Dia.
Power: 0.6HP
MRR: 1.96 in³
Torque: 0.84 ft-lb
Max Torque: 5.73 ft-lb
Cutting Force: 40.4 lb
Deflection: 0.0022 in
Max Deflection: 0.00500 in

And even with my derated numbers for the machine I'd still work into this carefully with the feed slider. And plenty of coolant. If I was trying this with my fogbuster I'd have it aimed carefully and be looking for good chips instantly, or stop. Welding a ton of chips to a nice YG-1 1/2" isn't a good time.

According to the calc there's no way no how for the 770 to take a full .6 DOC in 6061. It's miles short on HP. Low belt mode didn't make much difference. It's showing .17 for a realistic depth. It's just going to take several passes. And after that first pass the deeper you go the more difficult the chip evacuation and cooling will become. Maybe start with this for the first pass or two and then use less DOC for the remaining passes.

OR you could whip up an adaptive clearing tool path and work through the slot. This cut with a 5/16 end mill has almost the same MRR (material removal rate) it would be just as fast, but will take a little more time because of the brief moves to start the next pass as it walks through. It would go at the full DOC though:

Material: 6061-T6 Series Aluminum 95 HB
Tool: 0.312in 2FL HSS None Solid End Mill
Speed: 600.0 SFM/ 7337.6RPM
Feed: 0.0032 in/tooth 0.0065 in/rev 47.69 in/min
Chip Thickness: 0.0032 in
Reference Chip load: 0.0032 in
Engagement: DOC=0.60 in WOC=0.07 in
Effective Dia: 0.312 in
Cross Section: 0.42 x Dia.
Power: 0.6HP
MRR: 1.94 in³
Torque: 0.42 ft-lb
Max Torque: 1.40 ft-lb
Cutting Force: 32.1 lb
Deflection: 0.0013 in
Max Deflection: 0.00400 in

This has a much better chance of working though. Infinitely better chip evacuation, much lower torque, much longer tool life. I whipped up both in Fusion 360 for fun, about 2:36 to adaptive clear a 6" slot at .6" depth. The full slotting op with multiple depth passes was only a little faster at 2:13.

This NYC CNC video from 2016 shows the basics of how to set up a tool path like this:
https://www.youtube.com/watch?v=hGVf2GPqcv8

This is good practice for me. If my numbers are screwed up bad, someone here will be sure to set me straight.

[narrobb]

Only just starting to learn these calculators, so maybe I am using it wrong? Here is my screen shot. I derated the Machine itself to 1.1 ft-lb Max torque and 0.8HP.

I input the 0.6 DOC and then used the slider to adjust so all in the green, If I recall, I think it suggested 27 in/min then I put it down further. So does this mean even if all in the green, and the correct machine selected, the cut still can't be done?

0.2" DOC using same data did cut (but the cutting noise made me think its right at the top of the torque/load), while 0.1" DOC was much smoother and easy on the ears! I still have miles to cover, but perfectly happy with going for the 770 and not the 440 as was initially planned.

Thanks

[joshetect]

My 1100 wouldnt like a.6" DOC with a 1/2" endmill either.

The calculators can get you close, but not always, and you will always find things that may work on paper but not in real life. That cut will chatter badly. You also have to consider flute length, you need them to be above the cut so the chips can evacuate.

As time goes on you will figure out what the machine likes and doesnt.

Again, try it with a 1/4" endmill To get a good surface finish, you want to have a tool smaller than the slot you are making.

[narrobb]

Again, try it with a 1/4" endmill To get a good surface finish, you want to have a tool smaller than the slot you are making.

Thanks. Yes, if it was for an actual item, i will go that route, but as I am just making mess and learning I thought of experimenting with used endmils, i got over 80 such 1/2" endmils with half-life or so.

[joshetect]

Thats another thing to consider then, as the tool wears, it requires more from the machine to make the cut.

[mountaindew]

Thanks. Yes, if it was for an actual item, i will go that route, but as I am just making mess and learning I thought of experimenting with used endmils, i got over 80 such 1/2" endmils with half-life or so.

Just my opinion, want good consistent results, use good quality cutters. Try one of those cutters shown in your pictures then throw something like a 3/8 yg alum max cutter that Tormach sells and see the difference while it quietly plows thru aluminum while you talk on the phone.

I have some unknown cutters and even a few new ones in an old grizzly tool cutter set lol. Don't know exactly what they are good for as they do not cut anything well even wood . They do come in handy as alignment pins now and then.

[narrobb]

Agree about the cutters, hence my comment that even if newbie try the same feed/speed shown in various videos, milage may vary. As cutters brand/type/coating are variables.

However, those 100's of cutters I got in the auction (if thats what you are referring to in pictures) are almost 95% OSG, fully traceable, with manufacturer details online including speed/feed. For example, this one attached 59181 OSG cost $106. The other one is over $90 as well. And still sharp enough that if rotated between two fingers with almost no pressure it will shave some skin. I actually did not mention OSG or part numbers when i offered them up, and one person who received their 40 end-mils box replied back pointing to me how costly these bits are when new.

Just my opinion, want good consistent results, use good quality cutters. Try one of those cutters shown in your pictures then throw something like a 3/8 yg alum max cutter that Tormach sells and see the difference while it quietly plows thru aluminum while you talk on the phone.

I have some unknown cutters and even a few new ones in an old grizzly tool cutter set lol. Don't know exactly what they are good for as they do not cut anything well even wood . They do come in handy as alignment pins now and then.

[mountaindew]

Agree about the cutters, hence my comment that even if newbie try the same feed/speed shown in various videos, milage may vary. As cutters brand/type/coating are variables.

However, those 100's of cutters I got in the auction (if thats what you are referring to in pictures) are almost 95% OSG, fully traceable, with manufacturer details online including speed/feed. For example, this one attached 59181 OSG cost $106. The other one is over $90 as well. And still sharp enough that if rotated between two fingers with almost no pressure it will shave some skin. I actually did not mention OSG or part numbers when i offered them up, and one person who received their 40 end-mils box replied back pointing to me how costly these bits are when new.

I take that back
I have some 1/4" carbide up-cut and compression cut router bits from osg they are 10 years old and still put a clear finish on Acrylic.
I wont even admit what I paid for those at trade show prices even.