Help with my first project!

Coasters.c2d (95.1 KB)

Guys I need some help. Starting my first cut, a simple coaster project. The first operation is a pocket operation of some small squares. I have it set to be only 3/16" deep, in 1/2" material. I have zeroed to the probe, and the second time to the surface of the wood. Both times when it starts the first operation the 1/8" end mill drives straight down all the way through the 1/2" board and into the wasteboard. I stopped it before it did anything else so not sure what happens next. I have uploaded my Carbide Create file, can someone please take a look at it and tell me where I am going wrong? Any other criticisms would be welcome and appreciated as well.

Thanks

Hi @jburbs38,

From the g-code generated from your design file, there is no reason why the bit would try and dig all the way down to Australia, in fact the g-code preview confirms that it won’t go lower than 0.5" (which is consistent with what you set in the design/toolpaths)

I think your issue may come from incorrect zeroing procedure because the file is not fundamentally wrong (but more on this below). Can you describe how exactly you are zeroing, step by step and where you clicked ?

This being said, there are at least two potential problems with your design file:

  • the retract height is set to 4 inches, which is…way way too much (as show in the preview). Did you mean 4mm ? The retract height only need to be large enough to clear anything that can sit above the zero surface, like clamps. With 4" retract height, I’m surprised the Z axis does not hit the limit switch when retracting ?
  • the feeds and speeds are not right for a Shapeoko. Are you using an older version of Carbide Create?. In particular, the RPM of 6250 is not possible on a Shapeoko/trim router. I highly recommend you upgrade to the latest and greatest CC version, they fixed this weird behaviour where it would recommend Nomad-style feeds and speeds even when Shapeoko is selected in the setup. In acrylic (if this is indeed what you want to cut), you need to feed fast or you will get melting (all the more if you have a Dewalt router and its high minimum RPM value). Also your depth per pass could be increased to say half the endmill diameter, i.e. 0.0625 instead of 0.028, because no one wants to wait 87 minutes for this kind of simple cut.

EDIT: a personal recommandation for acrylic using the #102 is available here

EDIT: your project has “acrylic” as the material but re-reading your post, I doubt you are making acrylic coasters, so ignore those feeds and speeds above, and tell us what material you will be using

That’s 10.000RPM (assuming you have a Makita, that is min RPM), 47ipm, 0.0625" depth per pass
If you have a Dewalt, scale that up to 16500RPM (min Dewalt RPM), 77ipm, same 0.0625" depth per pass. Plungerate would be ~40% of feedrate, so somewhere between 20 and 40ipm

3 Likes

Can it be hitting the top limit and losing steps with his retract height set so high, causing his zero to then be off? I can’t remember if the z can still try to raise even with the limit switch there, unless it isn’t triggering for some reason.

2 Likes

I’m using Cherry, and my router is the carbide 3d router. Not sure how it got on acrylic, I checked that, must have happen when I was messing around trying tro figure it out. Carbide Create Build 431 is what I am using, just downloaded 433.

First ran the homing cycle, when that was done I cleared all offsets.

Zeoring was done first with the probe. I centered it over the target with the probe on the lower left corner, brought down the Z axis within 1/2" of the probe. Went to probe and followed the directionson thaty page. It touched the target, then touched each side. Then retracted back to the positon I started it from.

The second time, after homing the same way again, I lowered it down on to the corner using a piece of paper. When it touched the paper, I stopped and Zeroed All.

Then ran the file and it drilled straight through. I thought I was following the directions to the tea. I had them open and referred to them when needed. That last way I zeroed was exactly how I did it during my surfacing operation and that worked fine.

2 Likes

It did hit the z axis limit switch pretty hard, when I read that post a light bulb went off!

3 Likes

I fixed all of the above issues. Pretty sure the retract height is likely the problem. Have my total time down to 26 minutes or so. Its still telling me the speed for the .125" end mill is 10,000 RPM. I think the slowest the router will go is 12,000 RPM. I will run this after dinner and let you guys now. Thanks for the help.

5 Likes

Everything cut pretty well, except when it got to the profile cuts. My wood is 0.500" and I set the cut to 0.500". The first profile cut started where I expected it to but did not cut all the way through, left about 0.125" uncut. The other 3 profile cuts started above the wood, so that the first pass cut nothing. It then also left about 0.125 uncut.

I cut the coasters out and am continuing on, but just thought it was strange. Why is that happening?

a Z belt that is not tight can cause that (once you have a skip on the belt all Z is off after that)

yep, that or the Z pulley slipping on the motor shaft or the endmill slipping into the collet.

The end mill slipping into the collet was my first thought, so on my second attempt I tightened the collet a little extra. The result was not much different. It happen in about the same place both times, while cutting the profile on the first coaster. As soon as I can I will try to tighten to Z belt and see what happens. You guys are awesome and I really appreiate it. I hope (and beleive) that eventually I will pay it forward, and help out the next newb that has issues. Thanks

2 Likes

I tightened the Z belt and was able to cut through on the profile cut. I did get through the entire project.

One issue I am having is that I am getting a ton of vibration, to the point where I have ruined several pieces of wood when it vibrated out from the clamps. My clamps where as tight as I could get it and still several times it vibrated out of them.

Can someone give me some idea of where this vibration might be coming from and possible fixes for it?

Ouch. Can you share the feeds and speeds you used for that cut, for a quick check that they are within the “reasonable” range ?
Endmill size & number of flutes, router dial setting, feedrate, depth per pass, and material.

EDIT : or let’s do it the other way around. If I understand correctly you are cutting Cherry, using a 1/8" endmill which I will assume is a 2-flute. If you run your router at min RPM (say 12000RPM), I would recommend:

  • a feedrate or 24 ipm
  • a depth per pass of 1/16"

These are conservative settings, if you still get severe vibrations, something is probably wrong mechanically. Make sure to minimize the endmill stickout in the collet too (while still keeping enough length to be able to reach your total depth of cut, of course)

EDIT: I see you original design file has a mix of toolpaths with 1/8" endmills and 1/4" endmills. For the 1/4" toolpaths, assuming the 1/4" endmill you are using is Carbide 3D’s 3-flute (#201), I would use 12000RPM, 36ipm, and 0.125" depth per pass

1 Like

I’m definately faster than that. My depth per pass is right on but I need to slow down the feedrate.

Is there a good feeds and speeds calculator you guys use, maybe something on the simpler side until I figure out what the hell I am doing?

one good video to watch is https://www.youtube.com/watch?v=cjoNGACBkks

Mine is included here (look for “FS_worksheet_basics.xls”) if you want to take a look (but I guess you will have to do a little bit of reading).
The easiest way is probably to install the latest beta version of Carbide Create, they have a fresh set of feeds and speeds for various combinations of cutters/materials, that you can start from with confidence.

EDIT: oh and yes, the whole set of @wmoy wisdom videos is referenced here:

That’s like feeds and speeds heaven for beginners, definitely check it out.

1 Like

I have been watching Winston Moy videos since before I bought the Shapeoko. He’s awesome and explains things so well. Again thanks for the help, and I will eventually be able to pay it forward.

1 Like

Just wanted to add that I’ve also had my end mill drill unexpectedly through the wood mid-job. Which is very frustrating when it’s a nice piece of hardwood! I think in my case it was also due to an overly aggressive federate for the router RPM – I imagine my end mill was trying to bite off more than it could chew, and got pulled into the wood as a result. Now I’m getting to the point where I can tell if I am close to the “danger zone” by the amount of chatter (vibration) and the size of the chips.

(By the way, I think a year’s access to G-Wizard probably easily pays for itself, in terms of the amount of expensive wood saved from bad feeds and speeds!)

Interestingly this seemed to happen more often with the stock collet I received with the machine, but haven’t had it happen nearly as often since I got the precision collets, so I may have been having an issue with end mill slippage as well.

This also happens when the wheels in my Z gantry get too gunked up with dust — which actually happens pretty damn often, especially when working with oily woods like padauk. It’s usually preceded by a “clunking” noise as the motor tries to push downward but gets stuck on something. I always have to disconnect and re-home the machine when that happens. I’m sure this is because I am running dirty, and when I get a dust boot the problem will go away :slight_smile:

1 Like

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