I can’t figure out how to create a 45 degree bevel in Carbide Create. Is this possible?
Here is a snippit of the piece and what i need to create. The stock is 1" thick and there are 2 sections that need a 45 degree bevel.
I have imported the vectors for the bottom and top of the piece, but I don’t understand how to model it out in carbide create. I have created the model in Fusion 360, yes i have a STL file, but i would think i wouldn’t need to use that, or rather i’d like to learn how to do it in carbide create. I’ve found the STL imports don’t work well, so i’m exporting the faces as a vector and laying those in carbide create.
Sorry I can’t share the files as it’s a propriety product.
Any help is appreciated.
Here is that same section with the vectors in create.
First off, it’s not going to be possible to cut this part w/o leaving uncut round areas next to the vertical fixtures on a 3-axis machine unless you use a fixture such as a “Donkey’s Ear” to mount the stock at an angle.
Second, if you have a 3D model, just export as an STL and then import it, then you can just do the 3D Roughing and Finishing toolpaths as noted above. It should work well if you set the scaling and thickness correctly. If it doesn’t, send the file in to firstname.lastname@example.org and we’ll do our best to look into this with you.
Third, if you want to do this sort of thing in Carbide Create you have to either create the ramped areas first and at an overly large size using the Angle feature (and scaling it to match), then fill in the areas at specific heights using Equal, or draw them up using a depth map.
yes i assumed there be some rounding, and that’s ok, i can work with that.
I’ll try the STL file again, it didn’t seem to like it very much when i tried before.
I figured just doing a ramp (bevel) wasn’t an overcomplicated function but i just can’t seem to figure it out. I thought i’d ask here quick, otherwise i’m happy to use one of the training sessions to dig into this particular use case.
Edit: well crap, my pro trial expired now it looks like. I just got my machine a week ago, but i had downloaded the software ahead of time to play around. I was trying to figure out if this would work in the software or if i needed to purchase another program like Vectric.
Write in to email@example.com to get a second trial.
Because a angled component will angle all sides of the shape, and you only want one edge angled, you need to build the angled component bigger than the final bevel & trim it off.
These are the vectors I will use to build the model.
The black circles represent the actual corners. Your stock is 1" thick, so I’ll guess the chamfers are 0.75". The 2 smaller red rectangles are 1.5" wide (double the chamfer size). Model those first as an angled component, 45°, 0.75 height, 0.25 base height,
Then model the larger vector, the outside shape minus the chamfers, Flat, 1" height, Max or Equal Merge Type.
Now subtract the smaller 3 rectangles to trim off the ends of the angled pieces.
Ok, great let me go give this a whirl.
Ok, that seemed to have worked, how do I control the 3D toolpaths, what i mean is that the roughing pass is doing the angles as expected, but when selecting the finishing pass it’s doing the whole piece, which i don’t need, i only need the angled pieces, which don’t have vectors to select, so i had to select by layer.
Again, i’m sure i’m doing something wrong
You will need to draw in geometry to limit the 3D toolpaths to the desired regions.
Alternately, consider using MeshCAM.
Here’s how I’d do it. Draw up a side view to determine where the tool need to cut.
Then use that as a guide to draw the boundary for the 3D finish cut.
For a 1/8" ball, I get about 0.044" offset to get the tool tangent to the chamfer, and 0.0625 against the wall.
Gotcha, essentially creating a bounding box.
I have Fusion 360, it’s just much more complicated on the toolpaths versus Create
This topic was automatically closed after 30 days. New replies are no longer allowed.