profile cuts on an inclined board

This forum is for general discussion regarding VCarve Pro
Post Reply
wilkigr
Vectric Craftsman
Posts: 261
Joined: Tue Oct 13, 2020 3:14 pm
Model of CNC Machine: Sienci Long Mill

profile cuts on an inclined board

Post by wilkigr »

I would like to cut a series of circles from a board so that the cuts are at a 10° angle. I cannot tilt the router, but I can tilt the material.

I could do this on my scroll saw or band saw, simply by tilting the table. But where is the fun in that?

I played with the moulding toolpath trying to create a "moulding" that was nothing more than an inclined piece of wood, then doing a series of profile cuts, checking the "project toolpath onto 3D model" box. That did not work. I assume that is because the moulding toolpath is not a 3D model.

Is there some way to accomplish this?

thank you

gregk
Vectric Staff
Posts: 373
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: profile cuts on an inclined board

Post by gregk »

You can add a zero plane and tilt it appropriately.

Greg K

wilkigr
Vectric Craftsman
Posts: 261
Joined: Tue Oct 13, 2020 3:14 pm
Model of CNC Machine: Sienci Long Mill

Re: profile cuts on an inclined board

Post by wilkigr »

Tks, Greg, but I am lost. I read an article on using the tilt feature and I am still lost. Here is what I did. I created the work space size as a 15" square. I drew a rectangle 15 x 15. I selected it and chose to create a zero plane. Now, according to the article that I read, I was to open the zero plane, click on the tilt button, then the anchor. Then, I was to choose two points in the plane, one that will be the pivot point and one that will be on the surface that will tilt. However, when I click on the square in the 2D view, as instructed, all that happens is that "movement" dots appear in the corners.

It seems to me that the basic problem is that I do not have a component or model on which the zero plan rests. I could be totally wrong, of course.

I would appreciate if you could point me to an article or tutorial on how to tilt the zero plane. The one that I found does not help.

Thank you

User avatar
Bob Jr
Vectric Wizard
Posts: 461
Joined: Thu Aug 13, 2009 2:13 am
Model of CNC Machine: Axiom, Shark

Re: profile cuts on an inclined board

Post by Bob Jr »

Will,
If you go here: viewtopic.php?f=41&t=34650&p=253016&hilit=BBQ#p253016
You will find an excellent tutorial by Todd on how to use a zero plane to create slanted grooves in a BBQ board. The portion that you need appears at about the one hour mark in the tutorial. It's really a slick method!
Bob
"Be accurate."
W. Tell

User avatar
adze_cnc
Vectric Wizard
Posts: 4327
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: profile cuts on an inclined board

Post by adze_cnc »

wilkigr: be aware that the video linked above is 1 hr 16 mins long. The "tilted zero plane" bit comes near the end with the BBQ cutting board.

I don't think a tilted zero-plane is really what you need. People should re-read the original post.

To emulate such a piece as described a being cut on a bandsaw with a tilted table, in the original post, you are going to need to tilt the material (not any model) relative to the bed of your machine instead. Necessarily that would entail creating a jig.

If you look at the circle cut by the bandsaw end on you'll find it'll look like a parallelogram. Laying the material flat on your machine bed you won't get the "undercut" of the parallelogram by any toolpath if this is a single-sided job (well, you might be able to emulate it with a dovetail bit). A double-sided job, perhaps, but the transition area would need tweaking.

I could be way wrong with the above if I've not fully understand the original post.

User avatar
scottp55
Vectric Wizard
Posts: 4713
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP11.5
Location: Kennebunkport, Maine, US

Re: profile cuts on an inclined board

Post by scottp55 »

+1 To what Steven(Adze) said.
I too thought about the tilted zero plane(and using it twice(??))...tilting material is simplest.
But then Just started sipping first coffee and rushing to get cuts started.
Of course 10 degree tilted jig using tilted Zero Plane would be good if making multiples.
Watch the Icon to tell when exactly on the edge, and when line is perfectly 90 and on the other edge.
I've learned my lesson well. You can't please everyone,so you have to please yourself
R.N.

User avatar
adze_cnc
Vectric Wizard
Posts: 4327
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: profile cuts on an inclined board

Post by adze_cnc »

Rethinking things (what else are bus rides for) belay all I said about a parallelogram profile. I was picturing a router bit moving around an inclined board rather than a fixed blade with the board rotating around. The profile will be tapezoidal.

I still say no tilted zero plane. If the inclination angle matches a v-bit then use a profile toolpath. If not use the chamfer toolpath (or chamfer gadget if your VCarve is too old). Possibly use a moulding toolpath depending on what you need.

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: profile cuts on an inclined board

Post by 4DThinker »

You might get close with the fluting toolpath which can ramp down then back up. You would need to calculate depth at start (high point) of each circle as well as cut depth including the slope and how deep into it you want to cut. If you are cutting through just add a little depth to be sure the bit makes it through all along the fluting vector.

In Aspire we can save the results of toolpaths as a 3D Model, then import it to use in cases like yours. I don't have the later versions of VCarve so I don't know if it has that feature.
circle on ramp 4D.jpg
4D
Attachments
circle on ramp 4D.crv
(374.5 KiB) Downloaded 45 times

wilkigr
Vectric Craftsman
Posts: 261
Joined: Tue Oct 13, 2020 3:14 pm
Model of CNC Machine: Sienci Long Mill

Re: profile cuts on an inclined board

Post by wilkigr »

I regret the length of this post, but I could not think any way to explain myself briefly.

Tks much, guys. Lots to think about. I did plan on tilting the material at a 10° angle to the machine bed.

Initially, I thought that I would then simply cut out the circle, setting Z0 at the low point of the material. I immediately saw several issues. First, as the router moved in a circle, it would be cutting at increasing depths. I figured the solution was to take very shallow cuts - cuts that would not be too deep for the bit or my machine when it was cutting at the highest point of the tilted material. Another option was to set Z0 at the highest point of the material. I would need to set the max cutting depth much more than the thickness of the material to cut through the material as it sloped down to the table. I would be cutting a lot of air. No problem, right? Wrong! The second problem, though, was what led me to my question. That problem was that, by the time I could cut through the lowest point in the material, I would be hitting the router collet on the uppermost part.

That was why, in ignorance, I asked about a way to tell the machine that the material was tilted. I equated this to a carving that I did in a dish. I carved the dish first, then carved the model inside it, telling VCP to project the toolpath onto the 3D model. VCP was able to carve the model a consistent depth in the bowl, as it had already carved the bowl.

In this project, I would not actually carve the "slanted" tool path, since the material would already be slanted. I just needed this slanted toolpath so that VCP could then cut the circle in the same way that it cut the model in the bowl. It would keep the bit at a consistent depth in the material, following the slant because I told it to project the toolpath onto the 3D modle - the inclined board.

Last night, though, (really in the wee hours of the morning) I realized that, even if you guys could tell me how to do this, it could not yield the results I am after. To explain, if I tilt the table of my bandsaw and cut a circle with the material flat on the table, I end up with circle that in side view is a "wedge". If the top diameter is, say, 10", the bottom diameter is smaller. Think a very shallow funnel, or as adze said, a trapezoid.

However, if there was a way to tell VCP that the material was slanted and I could actually cut a circle, the result would not be a "wedge". The top diameter and the bottom diameter would be the same. The bottom would simply be "shifted over" by the angle. It would be a parallelogram.

So, in short, I wasted your collective time, for which I apologize. It was still a good learning experience for me. I will watch the cutting board video again, since I did not quite get the idea the first time.

Thanks to all of you.

wilkigr
Vectric Craftsman
Posts: 261
Joined: Tue Oct 13, 2020 3:14 pm
Model of CNC Machine: Sienci Long Mill

Re: profile cuts on an inclined board

Post by wilkigr »

I was typing as you were 4D, so did not see your post. I will look at your file now. As I said, though, I believe that I was wrong in thinking that this could be done on a CNC.

User avatar
adze_cnc
Vectric Wizard
Posts: 4327
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: profile cuts on an inclined board

Post by adze_cnc »

wilkigr wrote:
Sat Sep 11, 2021 8:45 pm
The top diameter and the bottom diameter would be the same. The bottom would simply be "shifted over" by the angle. It would be a parallelogram.
In that case we're back to "can this be done flat or does the material need a cradle to tilt it 10 degrees relative to the bed of the machine?".

If cut flat then yes it would be a double-sided job. Attached are two files (within the one ZIP file as the board doesn't allow attaching Rhinoceros 3D files) to play with:
  1. tilted-10-deg.3dm : 3D model to import in VCarve of a tilted cylinder (arbitrarily 10 inches in diameter ; 1 inch thick ; tilt 10 degrees from the vertical)
  2. tilted-10-deg-geometry.dwg : 2D file containing circles for the top and bottom faces of the .3D file
The tilt is so shallow that any 3D finishing path is going to need a very small step-over amount to properly cut.

If material is tilted and held in a jig the, yes, the tilted zero-plane method will work for this. I'd suggest having the x,y datum (i.e. co-ordinate 0,0) to be in the centre of the material. You'd draw the 10 inch circle with a centre at that 0,0 point.

You'll need to know the z height of the material top as mounted on the jig at that 0,0 datum point. From there the tilted zero plane can be created. Then it's just a matter of making a 1 inch deep profile cut projected to the 3D model as in the cutting board video and 4DThinker's file.
Attachments
titled cylinder.zip
2D & 3D files ZIPped together. For use with material flat on the machine
(55.3 KiB) Downloaded 35 times

4DThinker
Vectric Wizard
Posts: 1701
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"

Re: profile cuts on an inclined board

Post by 4DThinker »

If you want to make a wedged circle, think upside down and use the moulding toolpath to cut the 80 degree (90-10) sloped edge.

4D

DrHookCustomCues
Posts: 4
Joined: Wed Sep 27, 2023 6:28 pm
Model of CNC Machine: 6090CNC

Re: profile cuts on an inclined board

Post by DrHookCustomCues »

I'm in the same boat., all I want to do is create. a 10 degree angle. on a temporary waste board. And then I want to cut. certain Geometric depths. like, .250. and have that depth the same across the width and the length of 10 degree board. I just can't get it done. I would appreciate any help. What I used was a 10 degree on the zero plane...
75 YearYoung DAV just tring to have fun

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: profile cuts on an inclined board

Post by rscrawford »

To emulate an angled cut on the bandsaw, you just need a tapered bit and cut on the flat. You can buy all kinds of tapered bits, 10 degrees isn't hard to find. Cut your circle first with an endmill (the size of the smallest dimension of the circle), then use a tapered bit to finish the cut giving you the taper you want on your circle.

This is the whole premise of the V-carve inlay. I was doing these inlays on the scrollsaw decades before I started doing them on the cnc. Then, I would tilt my table and stack the two pieces I wanted inlaid together. The table tilt would have to match the kerf of my scrollsaw blade, so that the top piece would drop down into the bottom cutout tightly. I made pretty intricate inlays on the scrollsaw, but WAY easier with a v-bit on the cnc!!
Russell Crawford
http://www.cherryleaf-rustle.com

Post Reply