Cutting Depth Issues (was What is the problem)

Hello every one, i have my shapeoko xxl since january and i di not have any problem until saturday when i start the machine and as it was cutting for boxs. Suddenly the machine change direction and drill a hole throught the box and try to move direction Y. i was lucky to be there because the fire almost caught when the machine was trying to move and the box was fixe. First i just tought that it was an error so i strated again on another place and the same thing happen. So i decided to throw everything i created in carbide create in the garbage to restart the box. that’s what i did today but the same thing happen again. Is iy a problem that happen often and what do i have to do to prevent this problem.

thank you in advance for your help. Have a good day.

p.s. sorry for my english i am french canadian and dont write very often in english.

Please post the .c2d file, generated G-code, and step-by-step notes on how you are securing your stock and setting zero relative to it, either here, or to support@carbide3d.com

here is the .c2d file: boite carre 4 par 6.c2d (39.5 KB)

and the g code: boite carre 4par6 bit 1-4.nc (428.5 KB)

Now if i understand good you want to know how i setting zero on the machine: i just put the machine at the right place then i set the zero all and it’s done. I hope it’s what tou want to know. thank you

1 Like
  • retract height 0.25" and stock depth 1.75". that’s cutting it a little close maybe, if your endmill is long (and it needs to be in order to cut very deep into the pocket for your box) you might max out your Z … once you hit the top of the Z, the next plunge down will go too deep

the F&S you use are a bit on the aggressive side but not insane

Preview seems okay:

as does the .c2d

I suspect the problem is caused by cutting this very deep, very narrow slot.

Try adding geometry to cut as a pocket down to tab depth as described at:

0.25" retract, 1.75" stock, endmill needs to stick out 1.5" or so… how much height does a non-HDZ shapeoko have? it feels like this is cutting it close?

1 Like

Wouldn’t this be an “if you can get into it, you can get out of it” sort of situation? Presumably whatever the clearance is on a stock machine, it is enough to fit the bit and stock under there to begin the cut in the first place, so it ought to clear it coming out. Seems like the worst that could happen is a stop against the top end, but it still should clear the stock.

this is where the retract height needs to be added.

And once you hit the top of the Z, and try to go further, the machine loses where it is and will consequently go deeper.

2 Likes

Yeah, that is certainly true, although I guess I’d expect some “…and then it made a horrible grinding noise and things went crazy” statement to go along with that. I’m on board with the “having trouble coming out of a deep slot” theory, although I suppose I’d expect some unpleasant noises then as well.

Of course, one would have to then be familiar with what constituted an “unpleasant noise” versus the general racket a stock setup makes in the first place. :slight_smile:

1 Like

Thank you every body for your help. If i make a recap, my retract height seems too small and my cut is so deep that the mill robably touch the side of my stock so the machine go crazy and lose the way it is suppose to go and do what ever she wants. Am i right

for the noise i did not notice a very hard noise but i was not beside the machine doing something else during the cut

Hi Stephane,

No, the 0.25" retract height you used it quite ok, what they are saying is that it is theoretically possible that due to the very deep cut, when the machine retracts by 0.25" above the surface (that is 1.75" above the wasteboard), the Z axis collides at the top: but I think you would have noticed that, since it would make a horrible noise at the beginning when starting the job.

Do you know if your problem happened while cutting the pocket toolpaths, or the “lid” toolpath, of the “toolpath 4” profile cut ?

I think your problem is the following: it seems that your are using the 1/4" endmill #201, and you try to cut a depth of 1.75", that’s 44.45mm, but as you can see on the picture of my #201 below, it’s impossible to go down to 1.75" because you need more length inside the colle/router than what is left:

I suspect that you had less than 1.75" sticking out of the collet, at the beginning of the cut was ok, but at some point the collet ended up crashing into the surface of your stock ! and then it sure goes crazy (and dangerous) from there.

You need an endmill with a longer reach for this job.

Also, apparemment tu es français, si tu préfères un coup de main dans notre langue natale, n’hésite pas à m’envoyer un message privé.

2 Likes

Or, split the offending part into two pieces, cut them separately and glue them together after the “deep cut” is finished (in two operations.) I call it making a “sandwich” of the thick piece.

2 Likes

O.k i understand thank you very much to every body.

I have to admit that the first time I ran my machine into the end stop (y axis in my case) and caused the belt to skip teeth, I didn’t realize that what happened. It took a couple more tries before I realized that my out-of-position carving was due to skipped teeth. I initially thought the noise was just the impact at the end of travel on the axis. Also, mine only skipped 1 or 2 teeth, so it wasn’t really a horrific noise. Thus, I can understand how someone could crash their machine & cause a belt to skip without realizing it, especially if they were working on something else as stefetjew stated.

2 Likes

you are right bwechols i have to be more careful from now

This. I just ran into this due to having my sweepy boot set too low. There is a very, very, very subtle deep “chunk” that I now realize was skipping a tooth on z. The crazy thing is that I heard it several times and paused the machine to sanity check, but after hitting start again, it would continue with no problem. I figured it was my imagination but when I put my next bit in, the floor of my pockets was off. I thought it was a zero-ing issue, but in fact it was due to my machine thinking it was lower than it was due to the skipped tooth/teeth, leading to my first bit cutting shallow.

I agree with others that this problem is likely the reverse: it’s hitting the top and skipping, thus thinking z is higher than it actually is.

@stefetjew one way to check: run your path in air with no bit, setting the zero much lower than you are typically doing with the bit (make sure on retract it doesn’t come near the z limit switch). Repeat this after setting your typical height, but also remove the bit so you can run in air without hitting anything. Compare the results, and without the router/spindle running you should be able to hear any subtle noise differences between these two cuts.

1 Like

Good idea i will check that. Thank you.

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.