Finishing toolpath offset strategy

This forum is for general discussion about Aspire
bcombs510
Posts: 27
Joined: Mon Jan 11, 2021 2:05 am
Model of CNC Machine: Axiom AR8

Finishing toolpath offset strategy

Post by bcombs510 »

Hello,

I enjoy making these bowls but I have a bit more handwork than I would like to after the cut on the CNC. I noticed that the finishing profile is doing something strange when it gets near the end of the toolpath. My machine was jerking all over the place, Z up and down, etc... So I took a closer look at the toolpath and I see this:
OffsetBN.jpg
The model is a simple oval shape with a profile like below. I used two rail sweep between the ovals to create the shape.
Oval.jpg
I'm doing the roughing pass with a 1/2" downcut endmill and then the finishing pass with a 1/4" ballnose. The top of the bowl comes out pretty well with just a little bit of ridges to sand out. That's a fine tradeoff because I can run the 1/4" ballnose a lot faster than 1/16" TBN where I get a smooth finish. However at the end of the cut is all the jagged lines. Is there anything I can do to the model to solve this?

Here is the finished product:
IMG_3641.JPEG
IMG_3644.JPEG
IMG_3645.JPEG
Any ideas are appreciated.

Thanks!
Brad

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: Finishing toolpath offset strategy

Post by SteveNelson46 »

Try adding a zero plane. Also, try avoiding vertical or near vertical cuts. The bit is using more of the side of the bit instead of the tip to cut.
Steve

User avatar
martin54
Vectric Archimage
Posts: 7339
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Finishing toolpath offset strategy

Post by martin54 »

As has been said add a zero plane, it helps in defining the material surface & can make a big difference with this sort of carve.
I would probably use a larger ball nose bit if it's just the bowl you are cutting, what stepover are you using for the 1/4" bit? Reducing the stepover might reduce the amount of sanding required. It is always a trade off with machining time V sanding time :lol: :lol:

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Finishing toolpath offset strategy

Post by adze_cnc »

You may also get better results using the Moulding Toolpath and setting its "Vary Stepover" setting.

bcombs510
Posts: 27
Joined: Mon Jan 11, 2021 2:05 am
Model of CNC Machine: Axiom AR8

Re: Finishing toolpath offset strategy

Post by bcombs510 »

Thanks, all!

I do have a zero plane already, but perhaps the settings are not correct?
ZeroPlane.jpg
Brad

ZipperHead55
Vectric Craftsman
Posts: 186
Joined: Fri Apr 04, 2014 2:21 am
Model of CNC Machine: Axiom AR4Pro+ and AR8Pro+
Location: Edmonton, Alberta, Canada

Re: Finishing toolpath offset strategy

Post by ZipperHead55 »

What is your modeling resolution? Also, did you check your vector that you created the component from (for extraneous nodes)?

If you want to increase the resolution of the model, you have to do that when you create a new project (ie it can't be changed after the fact). You need to hold down the Shift key when selecting "Create a New File" under "Startup Tasks". You will be presented with 2 more options (Extremely High and Maximum).

Allan

bcombs510
Posts: 27
Joined: Mon Jan 11, 2021 2:05 am
Model of CNC Machine: Axiom AR8

Re: Finishing toolpath offset strategy

Post by bcombs510 »

ZipperHead55 wrote:
Tue Apr 04, 2023 10:00 pm
What is your modeling resolution? Also, did you check your vector that you created the component from (for extraneous nodes)?

If you want to increase the resolution of the model, you have to do that when you create a new project (ie it can't be changed after the fact). You need to hold down the Shift key when selecting "Create a New File" under "Startup Tasks". You will be presented with 2 more options (Extremely High and Maximum).

Allan
Interesting, how is the option seen when creating a new file different than below? Also, no extra nodes in the vector.
Fin.jpg
Thanks!
Brad

ZipperHead55
Vectric Craftsman
Posts: 186
Joined: Fri Apr 04, 2014 2:21 am
Model of CNC Machine: Axiom AR4Pro+ and AR8Pro+
Location: Edmonton, Alberta, Canada

Re: Finishing toolpath offset strategy

Post by ZipperHead55 »

You are showing the Preview Simulation quality tab. The option is available only when creating a new file (the resolution that your model was made with initially won't change, so you would have to create the model/component again with the new settings).

Image

Image

User avatar
SteveNelson46
Vectric Wizard
Posts: 2282
Joined: Wed Jan 04, 2012 2:43 pm
Model of CNC Machine: Camaster Stinger 1
Location: Tucson, Az.

Re: Finishing toolpath offset strategy

Post by SteveNelson46 »

I agree with zipperhead55. However, when you have an existing file already open you can hold sown the shift key when you click on the job setup button and you will get the additional model resolutions options also. The caveat is that it will have no effect on models already in the project.
Steve

ZipperHead55
Vectric Craftsman
Posts: 186
Joined: Fri Apr 04, 2014 2:21 am
Model of CNC Machine: Axiom AR4Pro+ and AR8Pro+
Location: Edmonton, Alberta, Canada

Re: Finishing toolpath offset strategy

Post by ZipperHead55 »

SteveNelson46 wrote:
Tue Apr 04, 2023 11:35 pm
.... However, when you have an existing file already open you can hold sown the shift key when you click on the job setup button and you will get the additional model resolutions options also. The caveat is that it will have no effect on models already in the project.
I didn't know this! I know I've been cheesed off in the past when I realized too late that I had selected the default value, and created/imported models, and created a new file (with the correct model resolution) and copied/pasted all of the other elements, and basically started from scratch.

I really wish (and I've asked in the past) that the settings were persistent (ie it remembers the previous settings when creating a new document) or those "extra" options were available without the added effort. It seems a little ridiculous, in this era of terrabyte harddrives and 250MB+ STL files available, that the default setting is so low (aka Very High(x7)), and I'm sure that there have been a ton ( bunch?) of newbies who bought a fancy model only to have it look crappy, due to the user selecting what appears to be the "best" setting (ie when not holding down the shift key), and then question the abilities of the model creator. But I guess we must be saved from ourselves (which is the impression I get whenever this is broached in the forums, social media, etc, where, I am assuming, that users were selecting the highest settings (Extra High, and Maximum) using a 386 computer, running Win95 and a 64MB video card, etc etc, and then complaining that the fancy model (a cube) was freezing their computer.... ) by having to work extra hard to get these advanced settings.

User avatar
rscrawford
Vectric Wizard
Posts: 1102
Joined: Mon Jan 17, 2011 6:49 pm
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
Location: Wetaskiwin, Alberta
Contact:

Re: Finishing toolpath offset strategy

Post by rscrawford »

Never use a finishing toolpath when a moulding toolpath will do the same thing. With the finishing toolpath you are relying on the model, which is NOT a mathematical equation but instead is a set of voxels (3D pixels). Your toolpath follows those pixels, rather than following a curve.

With the moulding toolpath (using the same curve you used to make your model), you get a perfect cut every time. You can even vary the cut on the more vertical areas to improve those (something that is impossible with the finish toolpath).
Russell Crawford
http://www.cherryleaf-rustle.com

User avatar
dealguy11
Vectric Wizard
Posts: 2462
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: Finishing toolpath offset strategy

Post by dealguy11 »

To pile on, the issues you're seeing in the cut are pretty normal with an offset carving path on curves. As it goes around the curve, it "catches" different 3d pixels at different levels and jumps around as you've seen. Recreating the component with a higher resolution level can reduce the problem but will not completely eliminate it.

Before the moulding toolpath became available, I used to address this on curved moldings by cutting up and down the face with a raster cut rather than trying to use an offset cut. It was **very** slow but it didn't leave those little jumps. Now that the moulding toolpath is available, it uses a completely different approach to cutting these kinds of shapes and gives far better results.
Steve Godding
Not all who wander (or wonder) are lost

bcombs510
Posts: 27
Joined: Mon Jan 11, 2021 2:05 am
Model of CNC Machine: Axiom AR8

Re: Finishing toolpath offset strategy

Post by bcombs510 »

Lots of good info, thanks folks!

I will try recreating with the moulding toolpath and report back,

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5886
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Finishing toolpath offset strategy

Post by Rcnewcomb »

You may want to send a feature request to support@vectric.com for a toolpath to specifically handle near vertical sections of 3D objects. Other CAM packages refer to this as either waterline or pencil line toolpaths. The moulding toolpath is already supporting that behavior,
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 931
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: Finishing toolpath offset strategy

Post by Tex_Lawrence »

I sent my request for improvement into support@vectric.com ... again!
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

Post Reply