I am currently working on modeling a watch. I am running into issues when it comes to the lugs. This is what I am looking to recreate with the chamfer on an angle?
Here is how I am modeling it with no luck.
Any suggestions on how I can achieve the model like the pictures above would be greatly appreciated. Thank you.
Hi @Benjamin ,
You have probably seen our watch modeling video, which has a simple radius along with the lugs.
Your model is a bit more complicated since it has kind of a variable chamfer along the edge. What is really cool in Shapr3D is that you can select edges and faces by themselves and with the Scale or Move/Rotate tool they can be transformed. Have you tried those?
If moving the elements will not help, you can use the Sweep command where the rail is the un-chamfered edge of the lug and you can define the swept cross sections as you want.
I hope I could help, if not, upload please the model and I will make a short video about these ideas in de next days.
Best,
Thank you for your reply and feedback. I was able to achieve the chamfer on an angle by selecting the chamfer face and using the Move/Rotate tool - didn’t know that was possible until now!
I would like to blend the two with a smooth edge going down, like the original watch images I posted, however, they are not lining up when selecting the two edges. The end goal is to have the whole lug slope down just like the image. Thank you.
In this case I would model that out manually, by creating a sweep, and subtracting it from the body. This way you have great control over the shape of the transition.
Thanks for the suggestion @Istvan! Anyway, you can go into more detail/give an example? I would create a new face of the same sketch with a sweep then subtract it?
Something like this. The red is the path of the sweep on the front face, and the green is the profile on the left face (hidden on this pic).
I was able to model the lug as follows-
First I extruded the lug sideways but as a drawing twice as thick as I wanted the final lug. I drew the lug profile with a 180 arc at the end of it so that the cylindrical curve at the end would already be there.
Then I drew a top profile to cut the lug to the curving taper toward the end.
Then I put a uniform chamfer along the outer edge, around the rounded end.
At this point I looked at the side sketch plane and could see the line segments between the section of the chamfer that was a smoothly curved plane, and the section that was conical at the end of the lug. i carefully drew two lines on the plane that aligned exactly with these segments defining the conical section and made those into a sketch that encompassed the conical end of the side profile of the lug.
I used this profile to separate the rounded and partly conical tip from the rest of the lug as a separate body.
I now had the basic lug- with the tip of the lug separate, in the form of a half cylinder, and half cone- and an even chamfer running continuously from the main body of the lug and onto the part I separated.
Now you do the trick of rotating the chamfer… except you select both the top edge chamfer, and the now separate conical chamfer. And then invoke the rotate tool and rotate the chamfer enough to get the taper to a point on the top edge but not run out of room on the conical edge.
You will find that the Z axis rotation might give a smoother result.
Once I did that, I unioned the two pieces of the lug, and then I cut off the bottom ( that extra thickness i initially extruded so I could get a good conic section ) to match the final curve of the bottom of the lug and expose just a little over half of the cylindrical/conic bend at the end of the lug.
Initial extrusion with even chamfer
Actually- I initially forgot to cut the taper from the top before chamfering- so I undid this, cut the curving taper from the top first, then did the same amount of chamfer- you can see the lug is thick enough to give me a nearly 180 degree radius at the end- well past the desired thickness of the lug.
Then I drew the profile to accurately match the visible line segments at the start and end of the conical surface at the end- and booleaned both an intersection of this profile and subtracted this profile from the separated main body of the lug- essentially cutting off just the radii at the end of the lug as a single separate part.
Then I selected the top chamfer and the conic chamfer together and did the rotate trick. How well this works depends on how accurately you cut the conic section off the lug along the edges of its face. There may be a way to project the segment lines of the conic face to the plane to get perfect accuracy… I’m not sure.
Sorry about the repeated posts but this forum won’t let me attach more than one picture to a post as I’m new here.
In my first post you can see that I unioned the two bodies back together and I cut off the lower 40% or so in the curve you can see in the profile drawing above.
Ha! This is a very cool way of doing it! 
It’s not a perfect solution. Zoom in close enough and there is often a slight mismatch between the conic chamfer and the simple chamfer… but at the scale of a watch, it’s close enough for rendering and for printing. Something like this I would bring into FreeForm to resolve any parametric mishaps before going to tooling.
I tried to match both top and bottom, it came close. It shouldn’t take a lot of time to shape the forms I made to get it where you would need it.
I started off with the same outlay you had, then I rounded off the ends. Then I made 2 forms, made the first one then used the mirror tool to make the 2ed one .
![image|374x500, 50%]
(upload://j8BHgasvdFmcnaVSV5GaHG34HSo.jpeg)
Then take the 2 forms and move them in to the lug to the desired depth and subtract tool to make the form of the lug. Here is what I got
Hope this helps.
Thanks for the feedback everyone! I’m going to try the suggestions and see how they work out.
