Trouble CNCing imported STL

[tuxedokman]

Hey this is a first time post, I'm new to all of this and hope to be regular around here! But I'm having some trouble on my first solo project without tutorials.

I'm having issues with cncing my stls. There are weird errors that show up in the cuts and preview. I have a game boy that
I have modeled in solid works and outputted as an stl. I can import the file fine into aspire but when i create cuts the program
creates its own artifacts (not sure what the right term is for this in the cnc community).

Issue 1: There is a straight line that goes across the top of the part. for some reason the program tells the bit to lift up and
then come down where it should just cut a straight line.

Issue 2: The edge of the part has a 1/16" radius on the edge, the program looks like it adds that radius but then leaves a ledge
at the end, then i got to cut the profile out it leaves this edge in resulting in a weird radius then ledge. i was able to fix this by telling the program to cut -.015 in from the profile, but i would just rather have the machine cut to the edge of the file.

i have included images of what the program is telling me. i would post pictures of the cut but its just the same as what the digital image are showing.

Are these issue because i dont know how to use the program well enough yet? or are they normal and i just have to address them in clean up?

My main focus with cnc is going to be cutting my own 3D files. I'm a native 3D designer and want to learn how to properly cut my creations.

[TReischl]

A concept that you need to understand is that Vectric is sort of a "voxel" based system. It works on shades of gray (IIRC, about 256 total), each shade represents a depth if you will. That is why I call it a voxel system.

Anyway, that makes it digital rather than analog. Soooo, if there is a slight difference when doling out the voxels some could be on one level and others on a different one resulting in a step.

What can you do about it? You might try increasing the model resolution when you open a project in the vectric software.

Now then, on to the meat of the matter. That model has very little that needs to be machined as a 3d STL file. It is pretty much purely mechanical. As such I would do the modeling over in solid works, but pass vectors to the vectric software and tool path accordingly. It is what I do with Rhino, I love being able to really look at my model in real time and roll it around, etc, but when it is time to machine something mechanical, I pass vectors.

[adze_cnc]

I'd expect that it could all be done with 2D toolpaths (profile, pocket, moulding, and perhaps fluting). Not all 3D things are really 3D.

[tuxedokman]

Thank you guys for your input, having different view points help. After playing with it a few hours i'm able to fix some of the issues by using extra vector shapes. I was just hoping for an easier way to use existing stls, but i understand why using the native system in Vectric is best for some objects vs others. im still learning so i guess its just a matter of milage and knowledge of the program & object i want to machine.

[Adrian]

One thing to bear in mind is that it might be easier to toolpath an existing STL but the quality of it will be inferior to creating the 2D vectors and toolpaths not to mention that it will take an order of magnitude longer to machine as a 3D piece.

[adze_cnc]

You've modelled the piece in Solidworks so you have access to all the geometry needed to export into Aspire. Just use a Solidworks drawing view (plan view). Set the paper size to custom and no scaling (i.e. use 1:1). No need for an STL or OBJ file.

The problem you'll find is that exporting to a DWG file from Solidworks leaves many closed shapes as multiple vectors even if you tell Solidworks to save them as closed. That's why I usually get an IGS file from Solidworks. Import it into Rhino 3D and extract geometry from that.

[phill05]

Why not just draw and tool-path it in Aspire as 2d vectors?

Phill

[adze_cnc]

Because some people find drawing in other software to be easier. For example trimming and splitting curves in Rhino 3D is generally vastly superior to doing so in VCarve. Or they like the ability to fully visualize the model in 3D before creating the toopaths for the model.

[phill05]

Point taken everyone to their own but I have found it better to do the work in Aspire mostly you can build it up in Aspire view in 3d and make changes if needed and no messing about with stray vectors or converting from a different program, I come from a 2D / 3D Autocad working background and I know what happens importing a dxf or stl you still have a lot of work to do before your cutting.

There is almost everything you need in Aspire from start to finish and if you don't know how to do something you only have to ask on here and along come some very valuable users that know a different way to get you out of trouble.

Phill

[TReischl]

......I know what happens importing a dxf or stl you still have a lot of work to do before your cutting.
......
Phill

Hmmm, nope. I do virtually all of my design in Rhino. I have never had a "a lot of work to do" before cutting. If I did, I wouldn't be doing it that way.

There are some serious advantages working the way I do. Here is a big one:

A part similar to the one in this post, almost all straight forward pocketing except for that ramp on the lower right corner. One of the interesting things that Rhino can do is extract edges of surfaces, like the edges of the ramp. So just before I export the file to Aspire I extract those edges. It also has a command to that allows those edges to be forced into and X, Y or Z plane. So I do that, then offset them a bit.

The result is that when I come into Aspire I have all the vectors for the pocketing, profiling, the boundary I need to control cutting on the ramp and I have the stl model. It is a wonderful thing.

Tracing in Rhino is a flat out breeze. Easy to adjust, no selecting a node tool to do so.

Organic modeling is also very easy and extremely dynamic.

Don't get me wrong, look over there at my thumbnail and you will see I have been using this software for about 14 years and am still using it. That says something.

So what is it in Aspire that I like? Obviously the tool pathing is easy. Also the ability to add draft and smoothing is a biggie.