spiral - in toolpath

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
Post Reply
rmueller1
Posts: 5
Joined: Wed Mar 31, 2021 2:48 pm
Model of CNC Machine: home built

spiral - in toolpath

Post by rmueller1 »

I want to plane a large surface by starting at the outside perimeter and making conventional cuts with 40% of the tool diameter as I spiral in to the center. Or I would like to go up one outside edge with a conventional cut, off the edge and then over and down the opposite edge with a conventional cut, moving in each time until I reach center. Vcarve seems to only have paths that let me spiral out from the middle or go up and back on the same side which forces me to do one of 2 things I dont want, namely 1) to start planing by putting the entire 2 1/2 inch cutter down on the board or 2) to make alternating conventional and climb cuts.
Is there a way around this?

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: spiral - in toolpath

Post by Adrian »

You could create a rectangular spiral vector and use that for a profile toolpath either starting it off the edge or specifying a lead-in ramp at the beginning of the toolpath.

User avatar
mrmfwilson
Vectric Craftsman
Posts: 239
Joined: Thu May 31, 2012 6:49 pm
Model of CNC Machine: Legacy Arty 36
Location: Georgetown, TX

Re: spiral - in toolpath

Post by mrmfwilson »

You could just draw vectors where you want the tool center to be. Make each vector start point alternate ends. Then use a profile path and the Vector selection order to control the order from one side to another. Maybe someday we will get to have choice of how to cut a pocket. From the inside or outside. Seems simple but I haven’t tried to write the gadget so I don’t know how hard it would be.
Mr. Wilson
CenterLine Designs
Facebook - Centerline Designs

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: spiral - in toolpath

Post by SteveNelson46 »

I usually use a pocket toolpath to surface my SB but I have experimented with profile toolpaths. Here's a spiral I sometimes use for my 24" X 36" spoilboard. It uses a 1.25 EM with a 50% step over. I drew the spiral using the Corel Draw "Contour" tool and then cut and reconnected the corners in Aspire.
Attachments
Spiral SB resurface-1.25EM .02 DOC.crv
(30.5 KiB) Downloaded 116 times
Steve

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5887
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: spiral - in toolpath

Post by Rcnewcomb »

What problem are you trying to solve with the spiral toolpath vs the standard toolpaths? i.e. why does it matter?
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

User avatar
TReischl
Vectric Wizard
Posts: 4589
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: spiral - in toolpath

Post by TReischl »

Rcnewcomb wrote:
Mon Apr 19, 2021 7:38 pm
What problem are you trying to solve with the spiral toolpath vs the standard toolpaths? i.e. why does it matter?
Hmmm, I don't know what problem he is trying to solve, but I can share why I would like to see a spiral in option:

First off, I work from a vise(s) quite often. Secondly, most times the stock is already cut to finish width and length. To flatten the surface I would like to spiral in with a climb cut to avoid splintering out the edges.

Even when I am just flattening stock I am not keen about the splintering (I work a lot in soft wood) which happens on the edge and if I use a raster routine produces nasty strings which can clog up the dust collector in the most inconvenient spot imaginable.

Is it a big deal for me? Nah, not really. I have become good at creating the rectangular spirals I need over in the design software I use.

But it would be one of those "nice things to have".
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
jfederer
Vectric Wizard
Posts: 364
Joined: Tue Nov 27, 2018 1:09 am
Model of CNC Machine: CanCam D23M
Location: Horton Township Ontario Canada
Contact:

Re: spiral - in toolpath

Post by jfederer »

I agree with Ted, it would be a "nice to have". I flattened both the top and bottom of my current project, the base for a fountain sculpture. The edge splintering on the top didn't matter because it was followed up with a drive rail 3D wall. But the bottom does have noticeable splintering, and this is with end-grain Maple. An inward spiral would have prevented this.
LSP01418.jpg
Joe Federer

www.fabrikisto.com incl. Tailmaker software
www.federer.ca

rmueller1
Posts: 5
Joined: Wed Mar 31, 2021 2:48 pm
Model of CNC Machine: home built

Re: spiral - in toolpath

Post by rmueller1 »

Thanks for the replies
We are flattening large slabs for tabletops.The reason for wanting these paths is to avoid the two things I pointed out in my post. Putting the full diameter of a large bit down on the center of a surface may be fine for planing a soft spoilboard but you risk a burn or more catastrophic result on hard maple. You don't want to be doing any climb cutting. Working back and forth with a conventional cut on opposite sides with 40% of the diameter will leave a much nicer finish on the grain.
Since our tops are all different sizes, the approach we have opted for is to write an Excel spreadsheet which generates the g-code for any sized tabletop we input. Maybe someday this can be done in Vcarve.

User avatar
Adrian
Vectric Archimage
Posts: 14544
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: spiral - in toolpath

Post by Adrian »

If you are capable of writing a spreadsheet that generates g-code then have you considered creating a Vectric gadget to do what you want?

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: spiral - in toolpath

Post by adze_cnc »

rmueller1 wrote:
Tue Apr 20, 2021 12:49 pm
Putting the full diameter of a large bit down on the center of a surface...
"Ramp Plunge Moves" for pockets and "Add ramps to toolpath" for profiles?

rmueller1
Posts: 5
Joined: Wed Mar 31, 2021 2:48 pm
Model of CNC Machine: home built

Re: spiral - in toolpath

Post by rmueller1 »

I don’t know how to write gadgets but I can look into it. After 32 years as an actuary I can make a spreadsheet that will take out the trash

Post Reply