Question Stepcraft 840 not cutting to depth

Hello All,

I apologize if this is not the correct forum. I'm trying to diagnose (or get troubleshooting ideas) so that when I'm in front of the machine tomorrow I can try some suggestions. We are using a Stepcraft 840 to cut some guitar bodies out of 1.75" stock material. Currently we're using MDF so that we can make sure the gcode is correct and get our process down before spending money on nice wood.

Our issue is when the toolpath is run, the depth is incorrect. If I set the toolpath to cut to a depth of 1" it seems to only cut about 1/2" over the expected passes (8mm depth per pass and the tool really doesn't seem to move more than 2-4mm per pass - I haven't measured it exactly). I've tried recreating the toolpaths in VCarve in metric and imperial and the gcode it outputs appears to be correct. I went so far as to recreate the whole drawing in metric (was originally in imperial) to no avail. After we make a cut that doesn't cut as deep as we expect and "GOTO ZERO" the machine returns to the home position flawlessly, so I don't think it's losing depth because of a plunge speed issue or anything like that, but I'm brand new to using a CNC so maybe that is wrong?

Also, when I tested running some codes in MDI field to set the Z height from 0mm to 25.4mm the travel is exactly 1" so I don't think it's an issue with the step calibration.

Any troubleshooting thoughts would be greatly appreciated - I have about two hours with the machine tomorrow to figure out what's going on - if I don't solve tomorrow it will probably be a couple weeks before I can get more time with it. I've attached the GCode for just the neck pocket toolpath for your review. In this case the neck pocket should be cut to a depth of .625" (~15.88mm) but it appears to only be cutting to a depth of maybe .35"

Thanks!

Hi,

just some short comments from my side and hopefully other users have more ideas to help...

What spindle you are using? (Kress or...?)
What rpm?
What feed-rate in XYZ?
What CNC SW (UCCNC?

(1 = End Mill {9.53 mm}) Thats too much for a hobby machine I think.
I´m using 1-6mm in diameter with a 800W spindle (mostly not more that 3mm)

8mm per cut and a 9.53mm end mill...that totally out of range!
I´m very conservative I must say so with a 6mm end mill I would start with 0.5 - 1mm per cut and 800mm/min feed rate or lower.

What I think is that your machine is loosing steps since it is totally overloaded.

8 mm depth per pass on a Stepcraft! No way.

Yes, DocBrown is correct, crazy! I cut guitar stuff and my roughing passes are done at no more than 2 mm depth per pass. Take a look at this video in which I do a test cut using 5 mm end mills on the top side:



I had an electrical interference problem on the lower side using 6 mm end mills which caused a serious loss of Z steps but the spindle still ploughed on with probably 12 mm depth but I wouldn't recommend anything more than 2 or 3 mm and that's with a perfectly tuned Stepcraft and an industrial spindle.

You can find videos of test cuts on the guitar body sections here:

https://www.stepcraft-systems.com/en/forum/accessories/4125-industrial-quality-small-hf-spindle-from-stoneycnc

They were done using a 4 mm end mill with 1 mm depth per pass but 2 mm depth per pass will work. Also I go very conservative with Z plunge rates, no more than 120 mm/min. Treat the Steppi gently!

Doug

Thank you both very much. My friend who has the machine was the one who set the depth per pass... but I guess he's just as unfamiliar with it as I am! We ended up on a 1.25mm per pass depth and that seems to have resolved the issue.

If we were to go to a 1/4" 2-flue spiral up-cut bit for the control cavity (1.5" deep) and body profile (1.75" deep) would 1.25mm still be appropriate or do we need to step down a little (like to 1mm or less)?

CommandaZ wrote: Thank you both very much. My friend who has the machine was the one who set the depth per pass... but I guess he's just as unfamiliar with it as I am! We ended up on a 1.25mm per pass depth and that seems to have resolved the issue.

If we were to go to a 1/4" 2-flue spiral up-cut bit for the control cavity (1.5" deep) and body profile (1.75" deep) would 1.25mm still be appropriate or do we need to step down a little (like to 1mm or less)?

Hi CommandaZ

1.25 mm is absolutely fine. I didn't see which spindle you are using but I reckon 1.5 or even 2 mm will also be o.k. Best to simply set up a 'ploughing' toolpath to test on a scrap piece of timber to save ruining your stock. I did this and it paid off.

I started off using 4 flute bits for my timber cuts which generated very small chips (sawdust really) but was advised to use two flute bits on timber but you've already got that aspect covered. Don't vertical drill with end mills is the other tip. I blunted the 4 mm 4 flute flute end mill I used to cut the body sections shown in my videos by using it for drilling the dowel registration holes. It's difficult to believe that you can overheat and quickly blunt a solid tungsten carbide cutter bit just by doing some vertical drilling but I can confirm that it's possible.

Basically, the centre of the spinning bit is at zero velocity so end mills should always be run with a translation in the XY plane or else the bottom cutting face will overheat. It also compacts the spoil back down in the cut hole. You can work around this to some extent by using a smaller end mill than the hole diameter and describe an arc in the XY plane.

Doug

Awesome - thank you Doug. I don't have the machine at my home so getting the details will be a bit hard, but it sounds like we'll be alright. I appreciate you letting me know about the vertical drilling - I did have some concerns about that. I'll probably just buy a special drill bit for those purposes or something.