Acrylic Workholding

[HeyKoolAid (Mark)]

Hi there - I’m cutting 1/4" cast acrylic and am having a difficult time keeping the sheets in place during the milling. I’m using essential clamps in my threaded washboard, and my feeds/speeds are pretty conservative. pocketing is less an issue, but when I’m cutting out the contour, all goes south (depth per pass is .025"). Using a 1/4" o-flute upcut bit. Any thoughts/ideas would be greatly appreciated.

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

I use 2-way tape. This gives an added advantage that I can cut 0.002 - 0.003" deeper than the stock thickness without hitting the table.

[HeyKoolAid (Mark)]

Thanks Tod. I’ve tried this but still not having much luck.

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

Photos showing the difficulty you are having?

What size sheets are you trying to cut?

With what tooling?

[HeyKoolAid (Mark)]

Here’s what’s happening. And here are my settings. I’ve figured out the work holding, but it’s still getting jammed and going errant - specifically on the finishing pass (see toolpath settings in the photo). The sheet is 12x16.

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

My usual suggestion is to not cut slots (this of course assumes that the machine is in sound mechanical condition).

Add a bit of offset geometry and cut as a pocket down to tab height or use the nifty new Cutout geometry if it suits.

[HeyKoolAid (Mark)]

Not sure what you mean by pocketing down (on the outside cutout)? Also, what’s the new cutout geometry? Thanks.

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

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…

The Cutout toolpath is an option in the new beta:

Carbide Create Beta Downloads | Carbide 3D

[HeyKoolAid (Mark)]

Thank you. I don’t have CC Pro for the cutout toolpath, but will try the offset/pocket combo.

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

Cutout is not specific to Pro:

Build 843
New
Added a new “Cutout toolpath” that automatically determines if you need multiple offsets to avoid deep slotting. Cutout toolpaths will not load in prior versions.

[HeyKoolAid (Mark)]

I’ll try downloading the new version again. I tried the offset/pocket method and it worked beautifully… up until the final contour pass. Not sure what I’m doing wrong here. Should I just pocket all the way down or will it be an issue with no tabs?

Lastly (I hope) - will the cutout toolpath solve for this? Thanks again!

[HeyKoolAid (Mark)]

So, I tried using the new Cutout toolpath. Two questions: (1) Is there a way to produce tabs so my piece doesn’t go flying? (2) I notice if I set the breakthrough to anywhere less than -.1(ish) the simulation shows a full cut-through.

Thanks in advance.

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

1. There is a bug in the current implementation which is being worked on, until then, make the Cutout toolpath fall a bit short of the bottom by inputting a negative value, then finish with a Contour toolpath which starts at the bottom of that.
2. That’s the way the UI works (which I was confused by the first time I used it, which is why I missed that tabs didn’t work)

Attached as a v8 file for inspection.

cutout_example_v8.c2d (52 KB)

EDIT: Note that in the above I forgot that this was for acrylic, so as @jtclose pointed out, wrongly used a downcut tool which is only suited for wood — as always, check tooling and feeds and speeds before committing to a cut.

[jtclose (Jim Close)]

You are using a downcut bit, which is sending the hot acrylic to the bottom.
And you have a .250 DOC.

Try the Amana bits listed in the CC library and use the default values.

[HeyKoolAid (Mark)]

Thank you. Does the “wide” cutout type allow for a safer/more conservative cut?

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

Yes, that is exactly the intent of the Cutout toolpath.

[HeyKoolAid (Mark)]

I think this did the trick. Thank you!