Engraving a pattern on a flat surface

john_partridge

I have a rectangular part with a flat top surface on which I would like to engrave some lines (a logo imported from a .DXF file). I figured I would specify the profile of the engraving tip in a sketch that was perpendicular to the surface I want to engrave, and then use Sweep to have the tip's face follow the logo lines.

This doesn't create a correct model since in real life the tip is a 45 degree endmill and the groove it cuts would be rounded at the ends of the logo lines and where line ends meet. So I used Revolve to turn the tip profile into a cone shape and then tried to Sweep the cone shape but that didn't work; Onshape doesn't let me select the face of the cone in Sweep.

Am I doing something wrong or is there a better way of approaching this problem? I would like a solution that allows me to choose whatever engraving profile I want (maybe a 45 degree endmill, maybe a ball endmill, whatever) and have it follow whatever series of lines (logo patterns) I want. 

Ideas?

TimRice

Glad I could help. You are correct, there is no easy way to directly model this in Onshape. It could be done, though the time required may or may not be worth it for you. 

TimRice

@john_partridge
You got it! Parasolid does not like self intersecting and zero thickness geometry.

michael3424

That sounds like a good application for a FeatureScript.

When I've done that sort of thing for others to see, I use the sweep you mentioned and then do a revolve extrude cut at each end of the cut chain.

When doing this for myself to machine, I don't bother with the sweep or the end cuts - just lay down the curve on the part, input the chain into my CAM program, and do a contour cut with whatever end mill or cutter I'm using. 

TimRice

As long as you dont mind your document being public, you could link it here in the forums and we could try to help you solve the problem.

john_partridge

timrice, I appreciate the offer. Here's the link: https://cad.onshape.com/documents/902a584a36d3a8fe7c12831c/w/0441cf5198407a84a9150543/e/a1a82491a5166b0ed49e97a1

What I'm trying to do is create a V-shaped channel in the "Slab" part that follows the lines of the pentagon and of the "JP" logo inside the pentagon. The channel should be .25mm wide (i.e., at the surface of the slab). The engraving tool tip has a 45 degree angle so if I'm remembering my trigonometry correctly, the depth of the engraved channel should be .302mm.

For what it's worth, here's what I tried (but gave up on): 1) create circles of .25mm diameter at each of the vertices of the pentagon and of the logo. 2) add lines that are tangent to the circles to create an inner and outer "outline" of the main pattern. 3) create a plane .302mm above the surface. 4) project the lines of the pentagon and logo onto the new plane. 5) loft the outline to the projected lines. (This is the step I gave up on.)

Also, while I'm on the topic, I'd like to make a feature request for being able to sweep a shape. If I could sweep a cone the same shape as the engraving endmill, creating the engraving shape would be easy. Then I would be able to create a library of engraving features (logos, model numbers, names, etc.) that I could add with the boolean operator. Very handy. 

_Ðave_

@john_partridge +1 for your last request, there's many 4th and 5th axis cnc machiing situations where I could use this feature.

TimRice

@john_partridge
Please take a look at the "Onshape" branch in your document. I used a sweep along the pentagon path to create what I think was your design intent. Also, I was unsure what you meant by circles at the vertices of the pentagon. If you are intent on modeling all parts of the CAM process, I would suggest browsing the CAM section in the App Store: https://appstore.onshape.com/apps/CAM. Using these apps will allow you significantly more control over endmill sizes, paths, etc. 

john_partridge

@timrice
Yup, I took a look at what you did with the sweep - thanks! Unfortunately, that doesn't work for three reasons:
1. It leaves abrupt / angled corners instead of a rounded corner that would result from an engraving endmill taking the corner.
2. If the profile that you sweep is not perpendicular to the sweep path, then the groove will be narrower than the groove that would result from an engraving tool.
3. This is kind of the same as #1: the endpoints of lines will have a "spike" point shape (depending on the orientation of the profile that got swept) rather than the rounded shape of an engraving endmill.

What did you mean by "modeling all parts of the CAM process"? Are there other tools I should use in addition to Onshape for handling situations like this? I'm totally open to the idea but it never occurred to me that engraving would fall outside of Onshape's capabilities. I looked at the App Store page your referred to and didn't see anything that looked like it would work. Do you have a specific tool in mind?

Anyhow, I tried another approach. I used the Sketch / Slot operation on the sweep lines to give them some width, and then extruded the resulting shape to emboss the surface. It's hard to explain; here's a link to what I did: 
https://cad.onshape.com/documents/189303a4e166a0fd002e51d4/w/b259d5639737e4c36c863669/e/e1f6bb6c030ca6cba09a8d09

This isn't a satisfactory result either because the bottom of the extrusion is flat instead of coming to a point the way an engraving tool would. Also, as a practical matter, the number of shapes I had to select for extrusion was ridiculously large (i.e., dozens) when I tried this technique on some text I had made with a single line font (see the letters "Mo" in the example I linked to above).

I'm just about out of ideas - hopefully someone else has run into this before and figured it out.

TimRice

@john_partridge
If you are looking for curved corners you would instead have to add a radius to each corner of the path that the profile is being swept around. Take a look at the Onshape branch to see what I mean. The profile was constructed normal to the sweep line so it should be constant over the entire path.

As for the CAM apps, I was suggesting these if you would like to generate toolpaths etc. The type of engraving you are trying to accomplish is certainly within Onshape's capabilities.

john_partridge

#timrice, thanks! Yes, I see what you're saying about creating a profile that is normal to the sweep line - that achieves the desired effect of having the correct width over the entire path. 

As to adding a radius to each corner path, that doesn't match the design intent of having an engraving tool tip follow an engraving path but I agree it gives a more attractive result. 

I don't mean to be argumentative but as it currently stands, I conclude that there is no simple way in Onshape to model the shape of an engraved line as it would be fabricated by a CNC milling machine, given an arbitrary engraving path (in my case it was a logo) and an arbitrary engraving tip profile (in my case it was a 45 degree endmill).

For what it's worth, I think the most intuitive way of extending Onshape to support this kind of engraving would be to let Sweep operate on a shape (in my case a cone) and the shape could be easily created by applying Revolve to a profile of the engraving tip the milling machine would be using. 

Thanks again for your help. 

TimRice

Glad I could help. You are correct, there is no easy way to directly model this in Onshape. It could be done, though the time required may or may not be worth it for you. 

john_partridge

#timrice
I think I found another issue. Take a look at this test example:
https://cad.onshape.com/documents/44631903214749adb0d69dc8/w/27caecf6d7e29a2fa96df9a0/e/161ea60f528c5bc923520b2b

I'm applying Sweep to the first long segment of the "M" and it removes the material as one would expect. But if you double-click on the Sweep operation and start adding additional segments of the "M" to the list of edges, Sweep will fail. That is, it turns red and no longer operates. For some reason, adding that third segment makes it unhappy. I think it's because the path is taking too sharp a turn but I'm not sure.

TimRice

@john_partridge
I tried to open the document but it appears I do not have access to it. Without seeing the doc, it could a different geometry issue that is causing the sweep to fail as usually a tight corner radius is not a problem.

john_partridge

@timrice
Woops. Sorry about that. I ran out of storage capacity and deleted it but I've recreated it:
https://cad.onshape.com/documents/765b1ea37e85f9b4d443bdb2/w/93ad14ba399cf5a3e72bf700/e/e562b8acc740c622f337cd41

I experimented a bit and confirmed that the problem occurs if the width of the "engraving" profile is too wide to take a corner turn without intersecting with itself. You can see the issue if you add path segments to the list of edges in the Sweep operation.

Thanks for taking a look at it.

TimRice

@john_partridge
You got it! Parasolid does not like self intersecting and zero thickness geometry.

Scott_Tarr

Has there been any updates on this specific subject?  I'd like to create a solid model, in this case a cutting board, that has a groove all the way around it.  The groove will be cut on a CNC overarm router, so there will be a rotating tool following a path.  So I'd like the groove in the onshape part to be the same as I will get from the cutting operation.  I know I can do it with a handful of commands, but I'd like to see if there was any work on sweeping a solid thru another solid to remove material. 

TimRice

Here is a simple example. If you would like to generate toolpaths you will have to use a CAM app but you can approximate the result very easily.

https://cad.onshape.com/documents/1731effb53ffacc765fc2bdf/w/29cf53f09f33f09dcb69d3f8/e/a5824cf6fac3231e6fa2cd5d