Finishing toolpath offset strategy
Finishing toolpath offset strategy
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:
The model is a simple oval shape with a profile like below. I used two rail sweep between the ovals to create the shape.
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: Any ideas are appreciated.
Thanks!
Brad
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:
The model is a simple oval shape with a profile like below. I used two rail sweep between the ovals to create the shape.
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: Any ideas are appreciated.
Thanks!
Brad
- 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
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
- 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
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
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
- 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
You may also get better results using the Moulding Toolpath and setting its "Vary Stepover" setting.
Re: Finishing toolpath offset strategy
Thanks, all!
I do have a zero plane already, but perhaps the settings are not correct?
Brad
I do have a zero plane already, but perhaps the settings are not correct?
Brad
-
- 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
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
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
Re: Finishing toolpath offset strategy
Interesting, how is the option seen when creating a new file different than below? Also, no extra nodes in the vector.ZipperHead55 wrote: ↑Tue Apr 04, 2023 10:00 pmWhat 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
Thanks!
Brad
-
- 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
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).
- 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
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
-
- 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
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.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 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.
- 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
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).
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
http://www.cherryleaf-rustle.com
- 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
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.
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
Not all who wander (or wonder) are lost
Re: Finishing toolpath offset strategy
Lots of good info, thanks folks!
I will try recreating with the moulding toolpath and report back,
I will try recreating with the moulding toolpath and report back,
- 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
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
10 fingers in, 10 fingers out, another good day in the shop
- 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
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.
Now there's a man with an open mind – you can feel the breeze from here.