Carbide Create Pro angled surface

[profexorgeek (Justin)]

Hi all,
I’m designing a compact dice rolling tower that will be cut on a CNC and require minimal assembly. I am trying to figure out how to make a “forward angle”. I would like to design this as two mirrored pieces and just glue them together to create a sealed inside (see drawing). I have cut topo maps and am familiar with cutting 3D shapes from grayscale or STL. However, this seems like it should be simple and less “hacky” than generating a grayscale image in photoshop or modeling an STL in another application.

Here’s a diagram:

In the isometric cutaway sketch, you’ll see that the die is dropped in a hole in the top, bounces off two angled surfaces, and then is ejected in the front by an angled surface. This is the surface I’m struggling to create.

In the ortho view, you can see that cutting the first two angles is easy since they are 90 degree cuts into the work material. But the final angle needs to ramp with a rough and finishing pass.

I could:

• Create a grayscale gradient in photoshop that results in a linear angle
• Create and import an STL file for the forward angle
• Use 3D shape components?

The first two seem hacky but I can’t make sense of the 3D shapes. I would assume I could create a round shape in “subtract” mode and subtract it from the work material but this results in no 3D preview and a toolpath that cuts all the way through the work material.

Is there an easier way to do this?

[WillAdams (William Adams (Carbide 3D))]

To do this using 3D shape components you have to create geometry larger than expected:

Use that to model the angle:

Then either restore or cut away what is not wanted:

[profexorgeek (Justin)]

It’s not obvious what is happening in those screenshots without a deep understanding of what the 3D shape properties do. I get the general idea that you are making an oversized, additive wedge shape and somehow stacking a flat surface component. But even if I fully understood this, it feels unscientific compared to parametric modeling I’m used to from 3D printing. For example if I wanted a 27 degree angle, I’d have to do some mental gymnastics to figure that out. For this project I think I will just cut the wedge in X/Y space and glue it in during the finishing process.

My most costly part of the production cycle is the product development so rapid iteration and predictability are critical. Reducing the most expensive human time will help adoption of the Pro version of the product. Here are some areas where the Create Pro feedback loop is unpredictable and time-consuming:

1. If you import an STL or grayscale image, you can’t change the settings or move it. If you change your material size (which is very common when planning a job or new product), the heightmap/STL file cannot be moved and must be deleted and recreated. Since you also can’t edit it, you have to manually record the settings you used before you finished the import process. This is an enormous time tax when setting up topographic or STL cuts.
2. STL files cannot be consistently imported with predictable Z scaling. When importing, you must scale X and Y to your material. Then you must set the base height and STL height separately, which destroys the scale relationship between the Z dimension and the X/Y dimensions. This makes sense in a heightmap where it has no absolute definition of Z scale. It does not make sense in an STL file where the relationship between Z dimension and X/Y dimensions is known. This is compounded by the fact that once you exit the initial import screen, you can never edit those settings again.
3. The 3D preview in the STL/Grayscale import does not allow you to choose material and defaults to aluminum, which shows dimension poorly. This 3D view also does not show you any other toolpaths. So, you can eyeball the preview and complete the import. But if you find that it doesn’t look right in the actual toolpath simulation you can’t edit it. So again, you must completely delete and re-import the STL or heightmap.

I understand that Carbide Create isn’t trying to be a parametric modeling program but these changes would eliminate major friction points in the workflow:

1. Allow re-entry into the initial import screens so you can change your settings without deleting and recreating components. I don’t understand why editing the settings after the initial import is entirely different.
2. Allow dragging of grayscale heightmaps or STLs in X/Y space.
3. Allow fixed Z scaling based on the X/Y scaling of an STL and render the red warning the way you currently do. This allows you to preserve the axis scale relationships and change your material Z thickness to accommodate the X/Y dimension you want.
4. Show the same orthographic tooling previews that Carbide Motion offers in Carbide create so you can see axis-aligned, orthographic tool paths. It’s incredibly frustrating to realize a toolpath dips off the edge of the material when you’re all set up to cut in the shop because the Motion preview offers insight that the authoring program does not.
5. Allow changing material in the 3D preview on STL/Grayscale imports.

If there is a better place for me to log these issues, and if all or part of these applications are OSS, please let me know! I’m the product manager for a large application by trade and work with many developers that contribute to OSS.

[WillAdams (William Adams (Carbide 3D))]

1. You can change any of the settings in the STL import window

2. Z is set independently of XY scaling and may be set to any dimension which one wants.

3. You can set the 3D preview to use any of the material choices from the Toolpath 3D preview.

See:

Creating a project from an STL file

as requested on support… Given an STL file: [image] which one wants to cut out as: [image] one first loads it into Carbide Create Pro: [image] which previews in 3D as expected: [image] When an STL is imported, the perimeter will be traced: [image] Assuming one wants to cut around the 3D object, one offsets from this by endmill diameter plus 10% or so: [image] [image] It is then possible to assign a 3D roughing toolpath using this offset geometry: [image] [image] Then a 3…

[Tod1d (Tod (with 1 'd'))]

@WillAdams

You can set the 3D preview to use any of the material choices from the Toolpath 3D preview.

Until you start adding more components, then it changes back to the default (Mine keeps switching back to Cherry, which is also too dark to see details).

The hardest/weirdest thing for me to grasp was that the 3D in CC Pro is not a geometric model, but a gradient bitmap / height map. And the tools were just geometric parameters to create the bitmap.

The next epiphany would be the vector you select for 3D toolpaths is just a boundary, and it cuts any/all 3D geometry within that boundary. So you can model what Will shows above, but only cut a portion of it.

You don’t have dimensions, so I’ll guess overall 3x3x6. I’ll start with a 12x12 workpiece knowing I need some extra space for the 3D model, and I still want to zero at the lower left corner of my actual stock.

Draw the pocket for the part with vertical walls

This is the actual box

Draw the rectangle to build your pyramid / model. I also added another rectangle to make a ledge to prevent the 3D toolpath from falling through the back of the box.

Model the pyramid. The angle doesn’t matter since it’s scaled. 2.75 is the 3" height minus the 1/4" back. The 0.25 base height starts the taper 1/4" above the table.

Make the ledge 0.25 high, and use the Merge Type: Equal. This will prevent the modeler from adding the edges that coincide.

Now design the 3D toolpath boundary. 1/8" offset from the inside wall of the box. 3D paths drive the tool ON the boundary, leaving the radius of the tool outside the boundary.

Mill out your main pocket

Rough & finish the angled surface using the boundary

I created a bogus toolpath outside to mill away the extra workpiece stock that really isn’t going to be there…

Leaving…

Justin_Dice_Box.c2d (72 KB)

[profexorgeek (Justin)]

This is very robust and helpful, thank you!

I did understand the concept that you only cut what lies within the bounds of the vector used for the toolpath. I use this on Topo maps and usually oversize them but keep the tool paths within a smaller vector so I get clean edges.

I think my biggest gripe with this system (coming from parametric modeling of geometric shapes) and hardest thing for me to understand is the lack of control over that face angle. From what I understand, you pretty much have to the angle and length of the hypotenuse manually based on the height of the cut and the scale of the grayscale image. And if you want a scoop (fillet-like) shape instead of a linear angle, you don’t have very precise control of the radius in Z space like you do in X/Y space.

I will experiment with this, thank you for taking the time to create such detailed instructions for my specific problem!

[Tod1d (Tod (with 1 'd'))]

Agree. And it’s not really made to do precise angles, radii, etc… But you can get close.
Best bet is to draw it up in a side view & transfer the dimensions, or do the math.