CNC'ed X3 speeds and feeds question

[Geekus]

I have an X3 which is CNC'ed with the following:

Gecko G540
1x KL34H295-43-8A, 906 oz-in (Z)
2x KL23H284-35-4B 387 oz-in (X and Y)
Deluxe kit from CNCFusion
48V 7.3A Power Supply

I really like the setup, but it is really slow. For example, I cut some profiles and pockets in a 5.5"x12" piece of 5/8" 6061 stock and it took about 7 hours total, I probably removed close to half the metal or more in the process with 3/8" and 1/4" endmills. I usually cut at 2000 RPM and am able to run the following speeds and feeds for hogging out the parts (most of these cuts would be full engagement slot cuts). I was using low pressure flood coolant for these cuts as well.

3/8 end mill - DOC 0.05" @ 7 ipm
1/4 end mill - DOC 0.0338" @ 12 ipm

Both tools are 3/8" shank with about 1" of stickout. I started with the values from G-Wizard and down rated the feed rates and sometimes the DOC to values which caused less complaining from the mill.

Do these values seem about right for an X3? I'd really like to get it going faster or deeper so I can spend less time on (what should be) small projects.

[dneisler]

If you do the pulley swap like I have posted on my website you get close to 6000 rpm and cut faster. I normally run a 3/8" FEM @ 42-48 IPM with good results.

[SCzEngrgGroup]

Not sure where you're getting your feeds and speeds. Even with your limited RPM, and with such shallow depth of cut, you should be feeding at least 2-3X that feedrate with a 2-flute cutter. With a 3 or 4-flute, faster still.

Regards,
Ray L.

[Geekus]

Not sure where you're getting your feeds and speeds. Even with your limited RPM, and with such shallow depth of cut, you should be feeding at least 2-3X that feedrate with a 2-flute cutter. With a 3 or 4-flute, faster still.

Regards,
Ray L.

Thanks for the info, it sounds like I have a problem somewhere. It is good to know it is not a problem inherent to the X3.

I forgot to mention that the 3/8 end mill is 2 flute and the 1/4 end mill is 4 flute.

[Geekus]

If you do the pulley swap like I have posted on my website you get close to 6000 rpm and cut faster. I normally run a 3/8" FEM @ 42-48 IPM with good results.

Thanks, that sounds like a great idea for an upgrade - do you have any pics of the conversion? Also would like to know if you had to do anything to keep the spindle happy (maintenance wise) for those speeds.

I think the spindle speed could be half the problem. I have seen my share of chip welding, even had it happen using coolant on my last project with a 4 flute 1/4" end mill running conservative cuts. Caught it before it clogged up and snapped, but can't seem to dislodge one chunk of aluminum from the end mill now so it may be a loss anyway.

I am going to look again at the tram and jibs to see if I can sort out the rest of the problem.

[SCzEngrgGroup]

Thanks, that sounds like a great idea for an upgrade - do you have any pics of the conversion? Also would like to know if you had to do anything to keep the spindle happy (maintenance wise) for those speeds.

I think the spindle speed could be half the problem. I have seen my share of chip welding, even had it happen using coolant on my last project with a 4 flute 1/4" end mill running conservative cuts. Caught it before it clogged up and snapped, but can't seem to dislodge one chunk of aluminum from the end mill now so it may be a loss anyway.

I am going to look again at the tram and jibs to see if I can sort out the rest of the problem.

Chip welding is a clear indication that your chipload is TOO low. When your chipload is low, the heat generating by cutting goes into the tool. When you run a proper chipload, the heat goes into the chips, and the tool remains cool. Plus, your tools will last MUCH longer! So, either reduce RPM, and/or increase feedrate, untl the chps are coming off hot, and the tool is remaining cool.

Regards,
Ray L.

[Geekus]

Chip welding is a clear indication that your chipload is TOO low. When your chipload is low, the heat generating by cutting goes into the tool. When you run a proper chipload, the heat goes into the chips, and the tool remains cool. Plus, your tools will last MUCH longer! So, either reduce RPM, and/or increase feedrate, untl the chps are coming off hot, and the tool is remaining cool.

Regards,
Ray L.

That's what I understood too, and it is really the problem I am having. When I have been man enough to go with the G-Wizard recommendation it usually ends with a broken endmill (if I am not quick)- not because the info is bad, but I suspect it has to do with my mill. Having broken quite a few by now I know that sound when things are going bad, and when I hear it I start dropping the feedrate in mach3 as quick as I can. If it is really bad I will go back in the CAM and drop the DOC as well.

After thinking more on it, I suspect that the flood coolant setup I have currently is the cause of the last chip welding - it does not blow the chips out of the cut so I have to do it manually (with a toothbrush ). Even so I am still running slower than recommended.

This is my less than ideal flood coolant - it runs on a fountain pump and barely lifts the coolant high enough to get it going:



A better pump is on the shopping list, but right now I cannot afford a little giant (I just spent as much as a new pump at my dogs vet tonight, the little rascal ate something she shouldn't have).

The finish has improved quite a bit with flood coolant though, which backs up the idea that the heat is not being removed by the chipload and is going into the work piece. Now I just need to determine why I cannot attain the recommended chip loads.

My first guess is to check the basics again which I will do this weekend (barring any work/home/dog problems). I will try some test cuts first with the 3/8 2flute and 1/4 4 flute end mills first and see how fast I can push them (using the G-Wizard roughing recommendation for feedrate and DOC as a goal) with a slot cut (maybe 1/4" deep?), and will crank the spindle up the the max speed which is around 2900 rpm. I will post the results here along with the G-wizard values for comparison. If anyone has other suggestions for a test I will try and do those as well (depending on my supply of scrap).

[SCzEngrgGroup]

You should always start with a shallow DOC, using the G-Wizard recommendations for RPM and feedrate. Then go gradually deeper, until you start running into trouble. When you get past a depth of about 1/2 the tool diameter, you'll have to reduce RPM and feedrate slightly as you go deeper. The numbers G-Wizard gives you are generally at the aggressive end of the scale, which you'll have trouble reaching on a small machine, especially if you're not using very high-quality tooling. Re-cuttng chips is ALWAYS a bad idea. Use an air gun to keep the chips away.

Regards,
Ray L.

[cornbinder23]

That's what I understood too, and it is really the problem I am having. When I have been man enough to go with the G-Wizard recommendation it usually ends with a broken endmill (if I am not quick)- not because the info is bad, but I suspect it has to do with my mill. Having broken quite a few by now I know that sound when things are going bad, and when I hear it I start dropping the feedrate in mach3 as quick as I can. If it is really bad I will go back in the CAM and drop the DOC as well.

IIRC in Gwizard you can adjust the HP rating of the machine a little bit lower to get a more conservative estimate of feeds/speeds.

JTCUSTOMS

[SCzEngrgGroup]

Adjusting the machine HP down only limits the peak MRR/power it will allow. For low-power cuts, like the ones here, that won't make any difference. There is a "gas pedal" control (down at the bottom of the G-Wizard window) that can be adjusted down to cause it to generate less aggressive estimates.

BTW - I am working on my own Feeds and Speeds calculator application, aimed more at hobby users. It will be similar to G-Wizard, though nowhere near as comprehensive (it will ONLY do feeds and speeds, not the many other things G-Wizard does). It will also calculate MRR, spindle power, do chip thinning compensation, etc., and adjust both SFPM(RPM) and chipload(feedrate) based on the material, tool material, depth and width of cut, and other factors. I will make it available free to folks here when it's ready.

Regards,
Ray L.

[cornbinder23]

Thanks for the clarification Himy!
I dont actually use Gwizard so I was kinda going from memory
I am looking forward to trying out your software. Do you have an estimate on when it will be available?
Sorry for the mis- info and jacking your thread Geekus

JTCUSTOMS

[SCzEngrgGroup]

I am looking forward to trying out your software. Do you have an estimate on when it will be available?

Should be in the next couple of weeks for the first, very rough, version.

Regards,
Ray L.