I am trying to create a case body for a wrist watch. I got stuck at a point while creating a cut. Attached is the image and part file for reference. Any help would be vary grateful.
Because there are four tabs I would only model one and then use the move/copy bodies tool to rotate one example of the tab, then mirror it about the center to generate the other two. You can use a revolve surface and split tool (or a revolve cut would work too) to get the sloping surface, then a variable fillet to generate the fading fillet feature. Then combine the bodies. The output is attached.
All you need to do is use your existing sketch & an Extrude Cut. It depends on what further work needs to be done but you should probably combine the 5 solid bodies first but it can be done as seperate bodies.
Note: you will need to increase the depth of Cut-Extrude2 as it's only partially complete (I increased it in bottom image).
I modified your sketch and did an revolved extrude cut and got a little closer to the screenshot you were showing. Maybe this helps
Thank you Kevin for giving your time. I know it can be cut this way but if you look closely on the drawing there is slope and hence there two dimensions for 4 and 4.93. If you have side view of then you will have only one arc and but the side view in the drawing shows two arc with end points at 4 and 4.93 respectively.
How did you get that revolve cut. Thanks in advance.
Originally because you modeled it as 5 bodies I wanted to use a surface and split all of the bodies, after I got into it I came to the conclusion that making one then copying it was a better idea - so a simple revolve cut would do the same thing as my revolved surface, split and delete bodies features. I basically made a surface that would divide the bodies, then used the split tool to separate the bodies, then delete bodies to remove the ones I did not want (the delete bodies step can actually be done within the split operation if you play with it). Like I said, a simple revolve cut would have done the same thing with a single feature - cleaner and simpler.
If you type "part reviewer" in the command search it will bring up a tool to step through the design of a part. It can be handy to see how someone went about creating something. Glad I could help!
Got it, initially didnt see the attached part file so asked for that, just saw the image only.
I'm curious. Why did you recommend the Move/Copy body feature and then a Mirror? Wouldn't two Mirrors be simpler and work just as well?
Let me start by saying there are ten ways to skin this cat, and mine is not right, or wrong.
I did that mostly because based on the existing geometry I am making the assumption that Jitendra is a relatively new user and not very familiar with the software (hence the reason the model has 5 bodies, and the model could probably be made from 1/4 as many features as it does). Using the move copy bodies tool, then a mirror that takes bodies on either side of the mirror plane is uncommon. It forces people to see less common modeling practices that may be useful down the road. Multi body part modeling can be a very useful tool that is (I think) never learned by most people. The same is true for the revolved surface, split, and delete bodies. It is not the fastest means to an end, but I bet he learned something... ;o )
I had a user the other day that was designing a weldment in the part environment and for every extrude he left a .0001 gap between the features to show them as separate bodies. He didn't realize he could just un-check "merge results" and get the same results with a lot less headache, and he was not familiar enough with the weldment tools in SW to actually make it out of a weldment... A little teaching can go a long way.
I'm sorry, I did not answer your second question. Yes, two mirrors would have done the same thing.
My bad, should of looked at the drawing a bit better.
That looks like dimensions for a variable chamfer? Starting at 0.93 & fading to nothing as it comes round & meets the body?
I tried variable chamfer but didnt get the same.
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