Well it may not be called a ramp. I ramp or slope the path I have Vcarve pro and carbide not sure what would work better. I just did a pocket to show the path but would like to tapper from front to the back where I did the pocket.
Knowing the terms is half the learning curve. 
That is a 3D pocket. I’d rough everything out at the highest depth using a flat end mill, profile cut the side walls with the flat end mill, then 3D pocket the “slope” using a ball end mill. There are, of course, other options too.
-Tom
Do you know of any tutorials that would show me how to do this?
I’m not sure; I don’t own Vectric. Check out the training section.
Watch the video the other day where they use the fluting toolpath. I haven’t actually done it myself and do not know if it would work. I’m pretty sure they grooved a drainage ramp on a cutting board.
Marty
Seems feasible in Carbide Create Pro…no exp with Vectric.
My $0.02 : Try defining your workpiece as a CC Model using the flat, Add options. Then select your curved vector and Subtract it using the Angle subtract option. You may get more facets than you want on the subtracted 3D shape, so Subtract those too.
-Mark
Are there other options using VCarve Pro? I and am trying to create a tool path to carve out a guitar neck pocket that is angled. At one end I want the pocket to be say 19/32" and at the other end 21/32", but I want a smooth slope. I tried creating 3 different rectangles at different depths and was surprised how deep a 1/32" cut actually is! It didn’t sand down smooth enough to work for me. Was hoping to see if this could be done easily in VCarve Pro.
Thanks!
It’s potentially possible to do what you are asking with the fluting toolpath, though it may require some math to account for tool geometry at that depth if the opening needs to be a specific size. At its simplest, you must draw each of the individual passes of the tool (multiple, side-by-side lines). This can be done fairly easily with the array copy tool, but if the cavity shape is irregular, it would create additional challenges.
Example of a basic slope using a Fluting toolpath, VCarve file included:
fluting-slope-example.crv (970 KB)
Realistically, it might make more sense to design the shape as a 3D model in another program, such as Fusion 360, and import it into VCarve. This would give you much tighter control since the software will use the model for reference, without all the extra math and dealing with 100s of stacked vectors. VCarve does not contain 3D modeling tools for creating these kinds of shapes natively, but its big brother Aspire does if that’s something you find you need down the road.
Thank you. The neck pocket I want to create is a simple rectangle so what you are suggesting shouldn’t be more difficult than what you show here. I will take a look and try this as Aspire is a ways out of my budget right now.
Thanks again.
Thank you. Not knowing what was called was the hard part.
You can do the design and CAM in Fusion. The size of your scallop (ridge between cuts) is dependent on your step over and the type of bit you use. I recommend a roughing pass using a flat end mill at 60% step over and then a finishing pass using a ball nose around 10% step over. You don’t need Aspire to get this done - Fusion can do it and I think Carbide Create can as well. Thought CC has had some items moved behind the paywall that makes it significantly less appealing (IMHO).
-Tom
I wonder if a simpler answer, instead of trying to wring something out of the software, wouldn’t be to make a platform at the angle you want your ramp, fasten your workpiece to it and just do a flat bottomed pocket tool path?
I tried this tonight. It actually worked great. Question though. Do I have to use a ball nose or could I use an end mill with a flute tool path? I started out carving a pocket to the shallowest depth I wanted with an end mill. Then I switched files and used your fluting tool path and carved out the same pocket going down to the deepest depth I wanted. However, I had to adjust the size of the flute vectors to fit in the original rectangular pocket. I am guessing because of the straight lines of the flute, the ball nose cuts on the center and half the width of the tool will go over if both lines are superimposed making the rectangle wider than the original pocket. Making it slightly smaller, this carve left slight ridges on the edges of the rectangle. This file also took around an hour to carve out. This is my first attempt with a fluting tool path so I can experiment but wondering if wiser CNC’rs have input on end mill vs ball nose for a flute.
Thanks again!
You can use any tool you like.
Yes, the tapered ball nose would be wider at the top. This is exactly what I was referring to when I mentioned accounting for tool geometry in my original post.
If you were to import a 3D model, you would have more control over the stepover (leaving bigger or smaller ridges) since it’s managed in the tool settings. But if you want to change the stepover with the fluting method, you would have to redraw the parallel lines at a different distance apart since it’s all manual.
