Make a watch case

morgan_blanck

Hi everybody! I am a pretty new user of  Onshape and is trying to make a watch case from a photo. I am a bit stuck and hopes that some can help me.

I started making a sketch of the side of the watch.



Then I extruded that and made a new sketch based on the watch front view.



I extrude that with the intersect feature I almost get what I want.


The problem is that the middle part gets bent downward as well, as can be seen in the following image.

 

Do anyone have a solution to my problem? I think that it might be better to make the lugs separate and then fasten them to a circle but I cant make that work either. So how would you guys make a watch case? Please link to tutorials that use the features I need to use if this has been discussed earlier 

Thanks in advance  

grochino

Hi @morgan_blanck
You can fix this by extruding the circular area again as an Extrude Add (instead of Intersect). First, close off the circular area in your sketch like in my image below. Then, create another Extrude feature, selecting the circular region, and Extrude Add.

Also, just a tip, adding the URL of your document to your post will help other users understand and help you with your issue  Let me know if you have any questions!

morgan_blanck

Thanks for such a fast response! It worked to extrude again, but now a new problem has emerged, I need to change the shape of the lugs. The outside looks good, but the inside does not as you can see in the picture below.


Here is the link to my document

https://cad.onshape.com/documents/bd08946adbb85fa8f10b144c/w/506814f06cc4e26052e077e0/e/a1874791818490483f63a9ef  

mahir

I think you should rethink the order of your features to minimize your feature tree while maintaining design intent. You were right to think about separating the lugs from the bezel. Try using multiple parts so you can more easily isolate areas of interest using merge scope.

1. Extrude the watch face as its own part. You can get the desired bottom shape with another simple extrude of your side profile, but I would modify the sketch to optionally remove the curved top portion (see upper corners below). That way the top of the bezel stays flat. 
   
   
2. Next, create one lug as a separate part. Get the side shape by using an extrude with the same side profile sketch above, but this time don't select the upper corner regions. Don't forget to select only the lug part in the merge scope. 
3. Get the other 3 lugs by mirroring twice.
4. Boolean the 5 parts together. This can also be done as part of the mirror features above