[narrobb]

Appreciate your take on this. I think I am going to do my first cut this weekend, probably in Steel if my order of flat 6061 did not arrive today.

This is probably not so much about cost (at around $65 single payment for 1HP for the 770 it does not hurt having it), but more about if you listen to the output without change.

I've read some posts/videos/comments that these calculators put out too aggressive results for the low powered (1HP) machines.

So do you follow the numbers exactly or do you dial it down a bit? If you dial down; which of the numbers you actually dial down (RPM, IPM, WOC, DOC?)

The other question (excuse a newbie machinist question); if the 770 motor is known to output the maximum Torque at a certain RPM, why not just set the RPM to that number on ALL cuts, and play with the other parameters?

Thanks

[MetalShavings]

Appreciate your take on this. I think I am going to do my first cut this weekend, probably in Steel if my order of flat 6061 did not arrive today.

This is probably not so much about cost (at around $65 single payment for 1HP for the 770 it does not hurt having it), but more about if you listen to the output without change.

I've read some posts/videos/comments that these calculators put out too aggressive results for the low powered (1HP) machines.

So do you follow the numbers exactly or do you dial it down a bit? If you dial down; which of the numbers you actually dial down (RPM, IPM, WOC, DOC?)

The other question (excuse a newbie machinist question); if the 770 motor is known to output the maximum Torque at a certain RPM, why not just set the RPM to that number on ALL cuts, and play with the other parameters?

Thanks

These are all questions I asked before I was afforded the opportunity to work with the HSMAdvisor software. I too own a 770 and it took me quite a while to figure out this software, let alone use it. Thanks to Eldar, the developer of the HSMAdvisor calculator I've manage to get it to work for me in the vast majority of cutting scenarios. The software has become very useful to me now but, nothing takes the place of hands on experience; which I don't have enough of.

I found that on my machine I could run it on the lower pulley for slightly more torque but, whether you use the upper or lower pulley both settings have their window of maximum torque. I've used the HSMA software to generate feeds and speeds using both the high or low setting on aluminum, various type of steel and stainless. I mainly use the faster/upper pulley just so I don't have to take the time to swap pulleys. For some reason I can't get myself to trust the WOCs that are automatically generated by this software when using my assigned DOCs. I've broken enough end mills doing this that in each case, even with the shallowest DOCs the pucker-factor is still quite high for me.

Something else I do that has nothing to do with feeds and speeds but more to do with speeding up the process of machining is, I'll set up all my tooling in their respective tool holders so they are all at exactly the same tool length offset. For me this really speeds things up. I do own the digial tool setter but this still seems just as fast for me. As far as generating overly aggressive feeds and speeds, I found this to be the case with this software; big time. In the HSMA software you can go in and edit the power rating of the 770 mill. It's rated at one horse power but, I edited this down to .75 horse power. I figured that If I could get the feeds and speeds recipes to come out on the conservative side I could then tweak those number upward until I got the kind of cuts and finish I was wanting. Before, when I tried the originally generated feeds and speed recipes, it cost me a lot more in broken end mills. It's much easier to tweak upward on an end mill that hasn't been ruined by being to aggressive.

There are also other features of this software that allows one to adjust feeds and speeds via some sliding scales and data input text fields that are quite helpful once you get the hang of them. It took me a while to learn just the little bit that I have learned using the HSMA software but, like I said, nothing beats hands on experience. It's that hands on experience that helped me make sense of the software and it was the workings of the software that helped me make sense of the hands on experience I've managed to get under my belt.

This is all old news to most of the seasoned machinist on this forum but, to guys like me who only uses my mill to run parts for selling on the internet about six times a year; plus oddball projects and stuff like that, it's taken me some time just to get this far.

MetalShaving

[SCzEngrgGroup]

For me, HSMAdvisor wins, hands down. VERY reliable, and has helped me greatly increase my throughput. GWizard (granted, I haven't used it in several years) often gave insane results, and different results at different times, for the same input. And it REQUIRES a network connection, REQUIRES Adobe Air (Yuck!), and seems like it wanted to do an update EVERY frickin' time I wanted to use it. NONE of those issues with HSMAdvisor. Eldar (the author of HSMAdvisor) also provides excellent support.

Regards,
Ray L.

[tmarks11]

+++1 for HSM Advisor.

[TurboStep]

Also +1 for HSM Advisor.

[mountaindew]

Also +1 for HSM Advisor.

Same here, simple install, simple updates, decent quick reference also. I used it to setup all the values for my preset operations library and my tools library. Now I just use it to check tools that stick out a mile for deflection and chatter.

[narrobb]

@MetalShaving, Thanks for taking the time. Great info. So it is aggressive (at least by 25%).

Also, thanks guys for the +1 but the question remains if you follow the output exactly or dial it down?

I did download the trial copy, it does need a bit of time to understand everything.

What would be a good conservative starting point?

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

Something like:

Steel: For Pocketing: 20 IPM, 0.05" DOC, xxx WOC
For Profiling:
for roughing:

Then Aluminum: ...etc.

Right now, I am looking at videos such as for NYC CNC and taking down the speed/feed they are using if it was for 770 and use similar type end mill.

[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.

[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.

[tmarks11]

I've read some posts/videos/comments that these calculators put out too aggressive results for the low powered (1HP) machines.

Nope. The author of both G-Wizard and HSM Advisor have Tormachs, and both software are written with modes specific to those machines.

thanks guys for the +1 but the question remains if you follow the output exactly or dial it down?

The answer is: it depends.

Are you going to use flood coolant or a mister? Use what it says.

If not using coolant and cutting steel: use what it says

If not using coolant and cutting aluminum, then you need to back it off, because the cutter can overheat and the aluminum weld to your cutter and then all hell will break lose.

The nice thing about cutting steel is you can tell when it is too fast. You want nice chips that are starting to turn blue. When they start turning dark blue or worse, then back-off your feed rate a bit, then your rpm a little bit. The not-so nice thing about aluminum is no visible indications of problem until the stir welding starts...

If you are going to dial it down, back off BOTH speed and feed proportionately (feed first, then speed), so you maintain the same chip load. Too little chip load makes the heating problem worse.

Or maintain the same DOC, but back off the WOC (obviously doesn't apply to slotting, where you have no choice but limit DOC).

The other question (excuse a newbie machinist question); if the 770 motor is known to output the maximum Torque at a certain RPM, why not just set the RPM to that number on ALL cuts, and play with the other parameters?

Because machining is all about the mathematics. Each material has an optimum SFM range to get best cutting performance and avoid destroying your endmills. Achieving that optimum SFM requires selecting the right RPM for the diameter of your endmill.

RPM = SFM *4 / D (where D = Diameter of your endmill)

Too fast for the material and you will burn up your endmill. Too slow and you will wear it out.

Once you have chosen your RPM, the next thing to determine is your feed rate to obtain the optimum chip load recommended by the tooling manufacturer to maximize tool life for the diameter of the cutter and the type of material. Too little CL overheats the cutter and kills endmill life (big chips pull more heat away from the endmill). Too aggressive a CL will cause excessive endmill deflection or will break it. Feed Rate is a function of CL and number of cutters (T) on the endmill

FR = RPM * T * CL

Once you have Feed Rate and RPM, then you chose DOC and WOC based upon the HP of the spindle. I am sure you will be surprised to know there are equations for that too.

Or you can just use HSM Advisor....

[narrobb]

Thanks Tim. Will be using Fog Buster. Gonna use HSM Advisor right from the start, but probably proportionally dial it little down initially as I learn this.

[tmarks11]

Thanks Tim. Will be using Fog Buster. Gonna use HSM Advisor right from the start, but probably proportionally dial it little down initially as I learn this.

Let me clarify a bit more. If a cut is too aggressive, then you should take action in the following order:
1. Reduce WOC (if contouring of facing) or DOC (if slotting). You generally want to keep full DOC when possible, since it makes use of more of the endmill, giving improved endmill life.
2. Reduce Feed and Speed proportionately.

DOC/WOC adjustments will reduce HP requirement, and reduce the heating of the endmill.

[narrobb]

Let me clarify a bit more. If a cut is too aggressive, then you should take action in the following order:
1. Reduce WOC (if contouring of facing) or DOC (if slotting). You generally want to keep full DOC when possible, since it makes use of more of the endmill, giving improved endmill life.
2. Reduce Feed and Speed proportionately.

DOC/WOC adjustments will reduce HP requirement, and reduce the heating of the endmill.

Thats great. Thanks

[Advil]

I want to be very careful not to over-bash on a good product here. I'm NOT a highly experienced machinist, I've just slowly worked at learning my Tormach for the last couple of years. Between G-Wizard and HSMAdvisor I will say that I have had massively better results with HSMAdvisor. GWizard I am convinced is an excellent tool on more powerful machines, but I have found that as so many other people have said it just frequently gives insane cut outputs for my Tormach. You have to almost always only use the far left position on the slider, even with the machine properly selected and even if you try to de-tune your HP ratings. I have never been able to reliably figure out why.

HSMAdvisor has both HP and Torque curves exposed to the user and has entries for both curves as well as separate machine choices for high and low belt settings. And the interface flows slightly differently when designing a cut. Much easier to understand in my book as it goes for a max DOC for good tool engagement by default and you can shallow it up as needed from there. Also, its ability to de-tune the HP, Torque, and IPM of the machine individually makes trusting the default "max" cut a situation where most of the time it works, unlike GWizard where most of the time it crashes a tool. Our machines generally never put out the full theoretical power even at the ideal point in the curve. Like Metalshavings said, I turn down HP and Torque max to 80% or 75%, and reduce the IPM max to 105 or so (on my 770) then I let it calculate the ideal chip thinning cut. From there I tweak it for tool life a little then try it. I'll usually enter it as provided with the slider in the middle at 100%, and start the program with feed turned down for the first go (as you should). Most of the time I'll be able to get the feed up to 100% and it really sings. HSMAdvisor has come up with some amazing numbers that work on 1018 steel for me. Conversely, usually with GWizard I have to use the farthest left slider position and STILL start the feed slow while holding my breath. I don't know why it always picks unholy overaggressive cuts but it has never felt like it is anywhere close to understanding the power limitations of the Tormach.

In GWizard's defense, it supports a few tool types that HSMAdvisor does not.

The other question (excuse a newbie machinist question); if the 770 motor is known to output the maximum Torque at a certain RPM, why not just set the RPM to that number on ALL cuts, and play with the other parameters?

Thanks

To some extent you can do exactly that with aluminum (with adequate cooling and lubrication) or soft steels dry air with coated tools. On a 770 Somewhere around 7000 RPM on high belt is the HP/Torque crossover. Sure, it's a good go-to, as long as you CAN use that much SFM with the tool you have chosen on the material your are cutting. Remember you have to cut a proper chip. If you are rubbing or not getting enough heat out or you don't have enough spindle power or rigidity to effectively go at that RPM, you have to go lower. Fortunately, if you want to cut hardened steel or titanium or other obnoxious materials (that I love cutting), you can just do it in low belt mode at around 1500-2000RPM. Some materials and tools need very low SFM like 200SFM or lower max or you are in for trouble.

There are many other masters here that can give you better more specific advice. This is just my experience from the last two years.

[brianbonedoc]

Love HSMADVISOR- also you get the full iPhone app version of FSwizard included

[SCzEngrgGroup]

NO feeds and speeds tool will give you perfect results every time. The whole point of these tools is to give you a starting point. You then have to fine-tune from there to find the optimal parameters for your particular machine, tooling, and job. You will, over time, develop a number of "standard cuts" for 90% of your work. But to get there, take what the tool gives you, and do some test cuts, starting out at perhaps 30% derating, then incrementally working your way up to see how close to the calculated numbers you can get. My experience has always been that HSMAdvisor, ,once properly setup for your machine, will get to very close. Sometimes your final numbers will be slightly less than calculated, and sometimes even more than calculate. But NO tool will give you optimal numbers every time.

When I first got HSMAdvisor, I used it a LOT. But I now have my library of tools and cuts optimized for my machine, and my normal workflow, so I rarely need it anymore, unless I'm working with a new material, or have a particular problem that has not come up before, due to unusual geometry, fixturing, or whatever. What I can say is that HSMAdvisor has saved me a TON of time, often getting the same job done in as little as 1/3 the time, and my average tool life has been increased considerably.

Regards,
Ray L.

[narrobb]

These are all great tips and information to new machinists! Highly appreciated.

I also just checked out HSMAdvisor CutCloud, looks interesting as a reference also.

[IMT]

I occasionally use Bryan Turner's free feeds and speeds calculator. Optimizing Feeds and Speeds Calculator for Milling
In my experience it works just as well as GWizard. As others pointed out these tools just get you in the ballpark, then you need to fine tune it from there.