Troubleshooting tooling marks and screeching specifically in one direction

[LHWQIB (H)]

Did a quick rectangle contour cutout today on some poplar and had some tool marks on the top side only:

3 sides the cut was smooth and humming but when it would turn the corner on the back edge it would screech and you can see the tooling marks.

Not a big deal but I’d love some ideas on what may have caused that specific side to give the cut trouble.

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

Did this happen when cutting a slot just as narrow as the tool?

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…

It may also help to switch toolpath direction — Carbide Create Pro has an option for this, or draw offset geometry to force it.

[jtclose (Jim Close)]

Looks like it was bouncing off the material. Was it a full depth cut ?

[gdon_2003 (Guy Donham)]

I saw a youtube video just last night about this subject. The explanation was about the lines are actually a couple of things. Tool deflection, wood fiber tearing and tool run out.

99% of Beginners Don’t Know This Easy CNC Trick!

[wmoy (Winston)]

It would help to know more details about your cut. Settings, endmill choice, and also what machine you have.

[LHWQIB (H)]

It was cut on Shapeoko 5 with 65mm VFD, workholding with tape + CA glue

1/4" downcut endmill, 2 flute, 1.25" cutting length

Cutting through 3/4" stock
Depth per pass: 0.130
Feed rate: 70.2
RPM: 19860

Good info so far guys will look into implementing. Let me know if something egregiously wrong with my parameters!

[No_Soup_For_You (Dean F***)]

something tells me this is another one of those straight flute posts. Or it’s tearout caused by how soft that wood is. Looks like I could put my finger through it.

[Tod1d (Tod (with 1 'd'))]

I like Will’s strategy of roughing a pocket leaving finish stock, then a full depth finish pass climb cutting to the nominal size.

However, the “depth first” pocket bug on narrow pockets prevents this from being as effective as it could be. You’re just wasting time on the 2nd pass for the pocket.

I would just offset the vectors by the 0.030" recommended in the video, and cut a slot with normal depth of cut, then cut the nominal vector with a full depth climb cutting pass.

[LHWQIB (H)]

Thanks for the feedback guys. A finishing pass at full depth of cut cleaned up all the noise along the sides.