[rs4race]

I'm really trying to cut down time to make some parts. So last night I gave trochoidal tool paths a shot with the deep DOC and low WOC. Go into FSWizard put in my parameters.

Material: 6061 aluminum
TOOL: 0.5 in dia, 2 flute, HSS, 1 in flute, 1.5 in stickout, 0.375 in shank.
Engagement: 0.375 in DOC, 0.05 in WOC, 4000RPM

It spits out 42IPM feed rate! Only 0.3 HP though, I thought it was a bit fast so I cut it to about 75%, 30IPM and thought F it, if I break something I will just fix it, its worth the experiment. Well that feed rate was just too fast. Either the spindle doesn't have enough torque, or it doesnt respond fast enough cause it would bog down pretty fast. I dialed it down to 40% feedrate (~12IPM) and it was a lot happier, but still would dip down to 3800RPM on some of the cuts mostly where it initially makes contact with the work piece, and stalled at one point where the cut was approaching that of a slot.

It cut down the time substantially though. As this operation took only 1 hour (even with slow rapids) vs 2 hours. For the next set I was thinking of switching to a 3/8" endmill and roughly same parameters 0.375 in DOC , 0.0375 in WOC, 4000RPM, maybe 20IPM. Or run the same 0.5 in endmill, and 0.25 in DOC, 0.05 in 15IPM.

Maybe my cuts are too aggressive? I didn't notice any chatter, so I'm suspicious that the spindle motor just isn't up to the task. Maybe there is a pot on the controller I can adjust (the motor gets pretty warm already though)? I really wouldn't mind upgrading it with something with some more oomph that I can interface with mach, maybe VFD controlled? I did some searching, and didn't get into the build threads, but it seems that most of the inquiry's don't provide any part numbers. I also looked on bf20.com/projects2 and most of the links were broken, but searched the part numbers and found them. Still I'm not sure what to go with.

What have you guys used to upgrade the spindle motor, what would you recommend? If you have something in your build thread please leave a reference.

[SCzEngrgGroup]

First, those feed rates are not too fast for doing real constant-engagement HSM milling. In fact, FSWizard is very conservative, as it does not do all the HSM corrections. If you want to see what is really possible, download the demo of HSMAdvisor, and see what it gives you. Your parameters give me 8280 RPM @ 155 IPM, which is about 0.6HP. Limiting to 4000 RPM brings the feed down to 75 IPM, and 0.3HP. And I can pretty much guarantee those numbers are correct - I've never gotten bad numbers from HSMAdvisor.

My standard constant engagement roughing cut in 6061 (on a Novakon Torus Pro) is a 1/2" HSS 2-flute, up to 1" DOC, 0.05" WOC, 5000RPM at 115 IPM. If I reduce the WOC to 0.025", I can run at 150 IPM. If I had a higher-RPM, higher-power spindle, I could switch to carbide tooling and really scream.

If your spindle is stalling, then, by definition, you don't have enough power. The right thing to do is reduce BOTH RPM and feedrate proportionally. Reducing only feedrate will reduce chipload, which will lead to the tool heating up.

Also what CAM are you using to generate the toolpaths? Unless it's a true constant-engagement HSM CAM (like HSMXpress), lead-ins, lead-outs, and corners will certainly be much heavier cuts, which will lead to stalling on entry as you've seen. A normal non-HSM CAM cannot be used to generate proper HSM toolpaths, as the strategy is VERY different.

Regards,
Ray L.

[rs4race]

Ray thanks for the input. I am using NX 9.0 with the trochoidal toolpaths. I was under the impression that trochoidal = HSM, but really didn't find a lot of information, except to run 10-20% tool diameter for WOC. I have a hard time finding what all of the parameters are meant for.. I see that HSMXpress is a free plugin for Solidworks so I will check that out. I have been using Inventor to model parts since I use it at work.

Are you suggesting the following model? Originally it was 70IPM at 4000RPM and I ended up running about 15IPM at 4000RPM. Roughly 21% so I should be looking at 840RPM? I appreciate your help, and downloading HSMXpress, and HSMadvisor as I type this.

[SCzEngrgGroup]

Ray thanks for the input. I am using NX 9.0 with the trochoidal toolpaths. I was under the impression that trochoidal = HSM, but really didn't find a lot of information, except to run 10-20% tool diameter for WOC. I have a hard time finding what all of the parameters are meant for.. I see that HSMXpress is a free plugin for Solidworks so I will check that out. I have been using Inventor to model parts since I use it at work.

Are you suggesting the following model? Originally it was 70IPM at 4000RPM and I ended up running about 15IPM at 4000RPM. Roughly 21% so I should be looking at 840RPM? I appreciate your help, and downloading HSMXpress, and HSMadvisor as I type this.

HSMXpress is also free for Inventor, so if you're already using Inventor, get that version (or maybe both!).

Trochoidal should mean HSM, but I'm not familiar with NX. The important thing is that the toolpath be defined so there is near constant engagement throughout the entire operation, with the option of reduced feed for plunge/helix/ramp moves where they cannot be avoided. When you run the code, the machine should make a nearly constant sound, with essentially constant load on the spindle, other than when it is cutting air (on the re-trace moves, etc.).

Yes, once you have the RPM and feed from HSMADvisor, if you need to adjust it more than perhaps 10%, you should reduce BOTH RPM and feed proportionally. The idea is to maintain a heavy chipload, which is essential to keeping the tool running cool - the hear is carried away by the chips. That said, in your case, the original numbers (4000 RPM, 70 IPM) seem wrong to me, so I would expect the scaled down numbers to be equally wrong. Try again using HSMAdvisor, and you'll get better numbers. Also be sure you setup a profile for your machine, especially RPM and power limits. Divide the manufacturers power rating by at least 2 or 3 to get a realistic number, then do test cuts to see where the limit really is. Remember the available power will be different at different RPMs as well.

Regards,
Ray L.

[rs4race]

Ok. Installing HSMXpress for Inventor as we speak. If I can figure it out I will try toolpaths from it this evening.

So in HSMAdvisor I plugged in the same parameters.
6061 Aluminum
0.5 in Dia, 2 flute, 1.5 in stickout, 1 in flute, HSS
0.375 in DOC , 0.05 in WOC, HSM box checked
4000RPM gives me 44IPM 0.3hp

I see speed and feed sliders, so I adjusted them equally (37%) until I reached 15IPM and it shows about 3600RPM , 15IPM, 0.1hp

Is this what your talking about? Thanks for helping me out.

[ChrisAttebery]

I generally use 4000-4500 rpm, 24-27ipm, .375WOC and .060 DOC. Roughly .68 cu in/min MAX. That's with the 1000W motor, not the 700W motor that came with the machine. I found that the stock motor was only good for about .25-.3HP. It sounds like you're just pushing it a bit too hard. I'd try running 24IPM, 4000RPM, .375DOC and start the WOC at .020. If that works increase the WOC or DOC in small increments.

You don't state what brand of tool you are using. Are they good end mills or cheap imports? I'm almost exclusively using YG HSS double ended end mills. I also stick to .375" and under unless I really need the extra DOC or I'm facing something. You also don't state if you are using coolant or not.

[ChrisAttebery]

I just looked at FS Wizard. I haven't used it in a few months. Basically, you need to stay around a MRR of .5 and around .2HP any more than that and you're going to stall the stock motor from what I remember.

[rs4race]

Thanks Chris I will give those settings a try keeping that hp range in mind. My 0.5in endmill is from grizzly, kind of a starter set. It seems to work great and leaves a good finish. no coolant, but an air nozzle to clear the chips. I think i might switch to 3/8 endmill.

I will check out your build thread but do you mind posting what your using for motor and controller?

[zero_divide]

Your cut is just too agressive for your spindle.
My suggestion is to mark the HP of the heaviest cut you can make and use that as your limit when making calculatios.

Also while coolant is not required when making light peripheral cuts, it will reduce friction and allow better metal removal rates especially on lower-powered spindles.
Regarding HSM and Chip Thinning with HSMAdvisor. I machine D2, aluminum, stainless etc with 150% feed override.
As long as you got the power, even default calculations made by my calcs are conservative comoaring to what you can really squeeze out of a machine.

Best thing to do when you run out of power is not to reduce the feedrate, but to reduce the depth of cut. When tou get too much rubbing, your Power consumption (relative to MRR) will actually be higher than when flying through material.

[rs4race]

Well using HSMAdviser and HSMXpress I am a lot happier than with NX. I probably wont go back. HSMXpress is so far easier to use and the toolpaths it generates seem a lot nicer, a lot less travel over already cut area, less rapids, and it has a mach3 post processor built in. Plus since its in Inventor I can change features and update the toolpaths with very little work.

I'm finishing a part that I started the other day and I'm just amazed at how much quicker its going. This operation requires a 0.25 in endmill. I put 0.25DOC 0.025WOC (10%) and was able to use the provided 26IPM at 3500RPM.

I would still like to upgrade the motor and controller with something in the 1hp range, maybe up to 6000rpm, 120v, and connect to my controller so mach can control spindle speed. I was looking at the kelinginc 1100w motor and controller recommended on bf20. Any recommendations?

[ChrisAttebery]

I'm using a 1000W motor off a PM30. I've had a couple "2+" HP 6000rpm treadmill motors and this one has more power and has lasted the longest. I'm running it with a KBMM-225 (220V) because I only have one 110V circuit in my garage and half of it's available power is already dedicated to lighting.