Better way to make this?

I figure there's some way to offset from the surface(s) but I couldn't figure it out, so I went the long way around.

https://grabcad.com/library/its-a-model-1

Answer
 
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6 Answers

The depth of the pocket is a constant .325"
I think you'd be able to just use the Cut-Extrude option with an Offset From Surface end condition.

Can you post your model? It will be easier to test one feature than remaking the whole model.

 
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Nice model.

As mentioned above the Cut-Extrude option appears to be the easiest.
However to increase the efficiency of this model you could use the Mirror function, and try reduce the Fillets/Chamfers into as few features as possible. If I was to make this model I'd try only make 1/2 or 1/4 of the model then mirror it. If done right you can reduce the number of features etx using this way.

Again as mentioned above without being able to view the model design it is impossible to tell which method would work best.

 
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Hi SM, the answers above are half right because if you want to select offset from surface you cant choose 2 separeta faces at the time like you have in your model, to make that you need to make a offset surface with o displacement an then when you make your sketch at the top you just select offset from surface select the offset surface that is going to select the two different angles and just put the measure of .375
I send you an example below

 
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It seems to me that the suggestions above do not respect the revolution shapes of your model. Because the cavity is a curve generation around the axis of the central cylinder, the simplest way is to generate a curved surface and to practice a removal of material "up to this surface". Just one fillet can be applied.

SW 2016

 
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You can finish the model with this technique and then count all the steps that you need to see if you have less features there, you have already 6 steps and only have just a half of the entire part.

 
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Yay, a 3D model to work with. Thanks for posting it.
Modifications are pretty straight forward:

1 Use the knit or offset surface command to create a new reference surface.

2. Edit the sketch plane for Sketch7. Right now it is in the "middle" of the new surface made in the last step, you want it to be above the part

3 Edit Sketch7. Those arcs in the middle of the profiles don't make any sense to me. Delete, or convert to construction lines. You could get into contour profiles, but I can't stand that "feature" it allows terrible sketches to be used when they should otherwise fail.

4 Edit Cut Extrude 4. The new end condition is Offset from surface. That surface is the one made back in step 1.

As Morgan suggested, you could clean up the feature tree a bit by designing with symmetry in mind.
The smallest feature tree is not always "best" though. It really comes down to how the model will be used/changed in the future.

Things I might do differently:
If cuts 1 and 2 are meant for standard hardware, make use of the hole wizard. to form those counter bores.

Wait until the end to add fillets and chamfers, unless they are really critical to the design.

Instead of repeating a series of features on the other side of the part, I would cut it in half, then mirror the part, but only if I knew the part would always be symmetric.

 
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