how not to overload (stall?) steppers on cnc 6040 router?

[j ferguson]

Somewhere on the web there must be advice on how to determine how much cut is possiblle in milling aluminum on a 6040 cnc router. But I can't figure out how to find it. And no, it may be Chinese but it's well made, and has performed quite well to date.

I think I've absorbed the guidance on figuring speeds and feeds, and not only that, I rented Bob Warfield's very comprehensive CNC G-Wizard. It appears that his algorithms are based in part on tool deflection limits. But on my machine, I suspect I could get stepper stalls before I bend the tool deflection anywhere near his limit. And worse, it could cause missed steps not to be detected until the next pass.

I've been cutting plywood to make ribs for r/c aircraft, formers too. It's worked brilliantly. I've also cut a lot of HDPE to make glue-up fixtures and that's worked well too. But now I need to cut some aluminum and am confounded by the question above. I suppose I could use half the step depth G-Wizard recommends and assume that will lighten the load enough to keep the steppers stepping. For example .010 steps instead of .025 seems good. And I have plenty of time, although at 75, maybe not all that much time.

Does this make sense to any of you and if so where should I loook?

 

[Boswell]

I use G-Wizard to get a Speed/Feed starting point and find that that if I follow it exactly then I tend to overheat when cutting aluminum and then of course the chips weld to the bit and ... I think that for me it is that I am not using flood coolant so I am probably not evacuating the chips fast enough and re-cutting, but regardless, I find that it is a good place to start and then I have learned out to de-rate it. Now to your question about stalling the steppers. First if you put too much load on a stepper it will just skip and loose steps will no longer be where you software thinks it is with all the consequences of that. In fact I think that the only way to really tell if you are loosing steps is to see the effect it has on the parts you are cutting. I am sure you could develop a test where you took deeper and deeper cuts measuring between each cut until you saw that you were no longer getting the measurements you expected. Also will steppers it is not just the load (speed of movement vs depth of cut/rpm but also the acceleration and De-acceleration. You could loose steps if you are just accelerating faster that the steppers can move the mass of the gantry.

Bottom line is that each setup is different and using tools like G-Wizard is great but you also have to mix that with experience on you router. You don't say what size cutter you are using, the RPMs. Is the .25 or .01 the Depth of the cutter is into the aluminum or the amount you are taking off on each pass? What are you using for chip removal?
Full disclosure: I am a self taught hobbiest and so your mileage may vary.

 

[JimDawson]

As you say, reducing the cut depth will help. The best advice I can give is to slow the feed down and maybe the acceleration. Steppers lose torque rapidly as the RPM increases. Cutting aluminum puts a lot more load on the steppers than light wood and HDPE. In aluminum, some kind of cutting fluid is very helpful also, I like kerosene, but WD40 works, as does just about any oil you have around.

 

[j ferguson]

I'm not sure what was lost here due to the crash, but I had posted a photo of my mister on the 6040. It's secured to the vacuum hose bracket which is used with the dust shoe - also hdpe. It's so easy to make really nice parts with hdpe. As to the dykem on the bracket - it's to show that I actually DO lay stuff out.

 

[coherent]

There are so many things that effect maximum cut speed that even for someone with another 6040 it's going to be a bit different. Each different end mill/cutter and it's sharpness is also going to effect the outcome. If everything is sharp, tuned and bearing/slides, screws lubed etc, the only thing you can do is run some tests to determine at what point you stall and back it off some cut depth, cut speed etc. Once you find the sweet spot, take some notes. I've always kept a binder with notes for any cnc machine I've had and refer to it when needed. Doing so really comes in handy if you cut something you don't cut regularly, or simply don't machine with it routinely enough to remember what works best for every material or bit. Or like us older folks the memory ain't what it used to be. I've personally found that while the feed and speed wizards are helpful and will get you in the general ballpark, there are huge differences between machines and capabilities when you start talking about smaller benchtop mills and routers. The difference isn't cutter capability and best performance settings for a specific cutter/end mill and material... (and that's what what the speed and feed wizard is calculating). The difference is machine capability variations. Machine capabilities aren't normally a governing factor with large industrial machine, but definitely are with small benchtop and home made or converted machines depending on spindle power, stepper size, linear rail and screw quality etc etc.

 

[spumco]

1. Get the torque curve (holding torque) for your stepper. Identify where the torque drops off significantly - probably somewhere around 500-750RPM, maybe a bit higher depending on the motor. If you have no idea who made your motor, find another manufacturer with a same-size (NEMA23?) motor that has about the same amps and use their torque curve.

2. Figure out your leadscrew pitch.

3. Pitch plus the motor torque will permit you to calculate the highest feedrate where your stepper still has decent torque.

4. Once you have this feed rate, you can use one of the feeds & speeds calculators (I prefer HSMAdvisor, but GWizard is OK too) and determine what the 'optimum' feed rate is with your spindle speed and about a 0.0015" chip thickness (feed per tooth).

I suspect there is a significant mismatch as the router spindle is spinning at about 20 million RPM, and the F&S calculator will tell you to drive the axis at 500 inches per minute. Not happening on that router (I think).

Compare that ideal feed rate to the motor torque chart, and you'll see that you'll have about 5-10% of maximum torque available. And when you command another step, the motor doesn't have the torque available to complete the step - missed steps.

5. You will see that at a feed rate with decent axis motor torque you're going to be taking a very, very thin chip. Rubbing, probably. So the solution is to reduce the depth & width of cut and raise the feed rate closer to the ideal. You stepper will have much less torque, but the reduced load means it won't (hopefully) lose steps.

Here's and example - you want to cut out a flat widget in a 1/4" plate of 6061-T6. You program a tool path to slot around the outside and any internal features. The slot should be about 0.010"-0.005" away from the final dimension (leaving stock). So far, so good.

For the initial slot(s), try ramping down with a very shallow pitch but at a higher enough feed rate that the tool is cutting and not rubbing. The tool walks around the part and slowly lowers in Z along the whole path. And program the slot in multiple depths:

Pass 1 - ramps from Z0 to Z-0.050" and then walks around entire contour at that depth
Pass 2 - ramps from Z-0.050" to Z-0.100 and does the same thing.
By pass 5 you're at the bottom.

Leave a couple 'thou at the bottom or some tabs to keep the part from flying off. Frankly, I'd use tabs maybe 0.010" thick 'cause I wouldn't trust an import router to hold +/- 0.001" or so Z dimension

Once it's done, you can take a clean-up pass exactly on dimension at full depth because the width of cut is very narrow - i.e. low tool pressure and the axis motor won't lose steps. Even though the tool is down in the slot you aren't cutting anything except that thin skin you left during the slotting operation.

Other suggestions:

1. Get an air blast or fogbuster type thing rigged up to clear chips and, more importantly, to stop chip welding.

2. Use sharp tools. Sharp tools reduce cutting pressure, thus lowering required axis motor torque at a given chip load and feed rate. HSS can sometimes be sharper than carbide. On the other hand, using special coatings (ZrN) can significantly reduce chip welding to the tool, and I don't know of HSS tools with ZrN coating - so you're back to carbide, maybe. I prefer carbide because it's stiffer, but I've got a wicked 1/2" HSS rougher that plows through aluminum for roughing passes.

3. If you can find radius corner tools, use them. Even just a 0.005" radius is better than dead-sharp. A sharp-corner end mill will dull in the corners, and a dull corner requires higher axis motor torque than a sharp radius corner end mill.

4. Consider using rougher or 'corn cob' tools if you can find them in the small sizes you probably need. The individual teeth penetrate the material more freely than a normal endmill - they simply cut with less tool pressure. If you need a better surface finish, do a second pass with a regular endmill to get rid of the cut lines the rougher left.

If you get the air blast thing rigged up you can stick with HSS and use really sharp tools.

This is, essentially, a long-winded repeat of what the other folks have suggested, but a bit of understanding why the stepper is losing steps at high speeds may help with future cuts.

 

[agfrvf]

Another thing to note the hotter the steppers get the less torque you have and more likely to skip. The longer you run the more heat soak you get.

 

[Boswell]

I have never heard about the heat causing missing steps. Many times I have run my Mill for 8 hours at a time and the steppers can get warm to the touch but I never had a problem with missing steps.

 

[j ferguson]

thank you all for your very thorough treatment of my problem. I'm on a trip and will respond in more detail when I get home.

John

 

[j ferguson]

I'm home. I have time to get into the torque curves for my steppers, and find some radiused cutters. Initially looking at corn-cob roughing mills, is it possible that they are intended for steel nad other harder materials not aluminum? Maybe I need to lookmore carefully.
Bob Warfield, of G-Wizard has just published a fairly extensive guide to cutting aluminum with a CNC router. It looks pretty good.

So thank you again, gentlemen. I think I have a path to get me to cutting aluminum with my 6040.

best regards,

John