Shapeoko 5 cutting wrong

[Timber_Forge (Curtis Bentley)]

Hi there, I am relatively new to using the Shapeoko 5 pro. The cuts I am doing into MDF seem to be not cutting correctly from the vectors made in carbide create.

The “est 1994” I understand was too small to cut correctly. However the other cuts are just wrong.

You can see in the picture above that the left leaf was cut correctly however the other two are very much not.

And why in the L T and E did it cut off parts of them.

I’ve tightened every bolt and screw, I’ve taken the cnc apart and sqaured it correctly. It’s almost as if the machine isnt reading the G code correctly or maybe I’m just missing something obvious. Does anyone have any insight of things I should check?

[WillAdams (William Adams (Carbide 3D))]

To confirm, the machine is mechanically sound, and the couplers are complete and properly secured? See:

The Support Show - Ep. 11 - Shapeoko 5 Pro Movement Guide

Are you cutting slots just as narrow as the tool? That results in near-constant high tooling engagement.

Where possible avoid slotting and add geometry and cut as a pocket

Making vacuum hose adapters

While cutting up vacuum extension wands for this is expedient, it’s a bit problematic given that Shop Vac recently filed for bankruptcy, was bought at the last minute, and production hasn’t caught up. I need a receptacle for the Sweepy 2.0 dust fitting — one option would be to purchase one from Woodcraft, but Carbide 3D sells blocks of HDPE: which looks to be just barely big enough for things to fit. Measuring the hose fitting I get a diameter of ~63.5mm — offsetting that twice we arrive at…

and/or

Adding geometry to cut as a pocket with a finishing pass

One technique which is often suggested to avoid slotting is to add geometry around a part which one wishes to cut out and cut as a pocket down to tab depth — here’s one technique for that. In this case, the project is a bevel gauge which will be cut out of 0.0625" (~1.5mm) thick aluminum: [bevelgauge] Due to the narrowness of the angles, an 0.03125" endmill has to be used, so after importing and scaling the file (we will be cutting out one which is 3") we select the perimeter and offset it tw…

and consider leaving a roughing clearance and taking a finishing pass.

Best Bit for full cut through

One which has a cutting flute length equal to or greater than the thickness of the stock — pretty much any tool should work. Big thing is the toolpaths — if cutting out, rather than just cutting a slot: [image] Offset to the outside by endmill diameter plus 10% or so: [image] [image] [image] Then cut as a pocket: [image] down to tab height or the penultimate pass: [image] then move the contour down to below the pocket and start cutting at the bottom of the pocket: [image] and…

[Chaotica (Joel McKenzie)]

What was your DOC & bit diameter for cutting this?
Looks to me like it was trying to go too deep too fast.

[SDGuy (Anthony)]

Post the file so we can look at it.

[Timber_Forge (Curtis Bentley)]

Thanks for all the responses!
I’ll give cutting as a pocket a try see if that changes anything. As for the depth of cut it was programmed to the default #102 1/8th endmill for soft wood, depth per pass was 0.03" to cutting through 0.5" MDF

[Timber_Forge (Curtis Bentley)]

The Walsh Family.c2d (516 KB)
This was the program

[Chaotica (Joel McKenzie)]

After looking at your project file, I would think the most likely culprit is the feed rate - 1/8" bits can get easily bogged down in the material trying to be pushed too quickly. Also, for small figure toolpaths, the spindle tends to ‘jerk’ around rather than smoothly maneuver when it is trying to move around too quickly.

Depth of Cut is really shallow - yet in the pics you posted it seemed like the bit was not reaching the same depth at the bottom of the cut. Was the bit properly wrenched tight into the collet?
If your machine mechanics are all tight(no slop/backlash/wiggle on any axis) & all your stepper motor connections are solid(a bad/poor connector can result in intermittent/random loss of steps…wiggling the connectors around while jogging the machine is a good way to find bad connectors), then I would focus on adjusting the feed rate down & ensuring the bit is not slipping & is square/tight in the collet. I would also turn on ramping in the program.

[Timber_Forge (Curtis Bentley)]

Cutting as pocket worked perfectly. I did some more tests and I definitly think it was feed rate for sure. I’ll do some more test but this was a big help. Thanks!