How can I cut/merge two objects (making a WROOMU out of a WROOMD)

[johnwYMVVZ]

I need a new step file for Eagle.  I found an existing step file for an ESP32 WROOMD (with onboard antenna) and I am trying to convert it to a WROOMU (u-fl connector for external antenna).  Several issues:

• I managed to cut a notch out, but would like to have new walls around the cut.  Not sure how to do that but join and intersect aren't getting it done.
• I need to insert another step file of the u-fl connector - how do I do that?
• How do I move the text down before cutting so it doesn't get chopped?  (it won't match the U but that's not a big deal.  It would just look better if it wasn't cut with the shell.)

I attached the STEP files so you can see what I'm working with.  Thanks for your help!

End result:

[ToddHarris7556 · Accepted solution]

I don't have the time to make a video walkthrough at the moment, but hopefully can offer a couple of quick points that might be helpful:

1) Assumption: No disrespect intended whatsoever, but it sounds like you might be coming more from an Eagle background than solid modeling. I'm guessing you really just want to get this part made, and have less interest in learning very much about modeling. All of the following is offered in that context.

2) Adding walls to your cutout: If you're really interested, you can look at the part and see how they made it, then try to model that. Caveat: If the 'walls' consist of a metal flange that is bent down, then modeling it accurately will involve at the very least some more advanced skills. The 'easy' way to approximate this would be to sketch a closed shape on the PCB, and EXTRUDE it up to close off the corner. Fillet the sharp edge at the top if you want it to look nice (note 'nice' is relative.... pleasing to the eye is not the same as satisfying a manufacturing engineer who will immediately recognize that the part can't be built). It depends what your objective is. 

3) Inserting another STEP file:

 - open both STEP files, and save them as Fusion models.

 - Close the User_Library_U file

 - in the Data Panel (left side of screen) User_Library_U file into the main assembly. It will come in as a linked component (icon with the little chain link in the browser) and you'll have the opportunity to drag it into rough position. Note that this includes pulling the base of the antenna part up to match the top of the PCB

  - If the rough position is good enough, export out as a new STEP file. If you want more accuracy, then create a joint to position the two parts, then save and export. 

4) Moving text: a little trickier, but not hard. The imported STEP file comes in as a series of individual bodies. (Conveniently named 'Body1, Body2, Body3' etc.) If you start selecting bodies, you're find that the cover, included all of the embossed text, is all one body. I would think the easiest approach is to SPLIT these. Basically, select the cover body, then use the top plane of the cover as the splitting plane. Everything above that will be split off into it's own body, which can then be manipulated independently. Yes, there are lots of them, but if you use a top view, window select them all, and MOVE them, it's easy. I'm sure there are also direct modeling ways to do this which might avoid creating all the independent bodies.  

[johnwYMVVZ]

I was a 3D Studio user back in the Yost Group and Discreet days, through 3DSMax 9.  I am definitely interested in learning more about modeling things correctly, and solving specific problems like this is the easiest way for me to learn.  I appreciate your insight.

It would be nice if I could select the 2 edges of the sketch rectangle I extruded to make the cut, as well as the top and side edges of the shell above and F360 would create a face that formed that back "wall" that I could fillet with a small radius to look like a fold.

I will try the rest of your suggestions.  Your end result is what I am trying to accomplish.

[ToddHarris7556]

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It would be nice if I could select the 2 edges of the sketch rectangle I extruded to make the cut, as well as the top and side edges of the shell above and F360 would create a face that formed that back "wall" that I could fillet with a small radius to look like a fold.

There are often multiple valid ways to solve modeling challenges - what you describe sounds workable:

- draw the rectangle

- extrude down to make the cut 

- extrude just those two edges down as surfaces (the visibility of the sketch will be off once you extruded down, but you can turn it back on. Make sure you're in DESIGN>SURFACE tab. Turn off chaining selection and select just the two edges you need using the CTRL key. Extrude down to the PCB surface to form the two walls, with no thickness.

- use DESIGN>SOLID>THICKEN to turn your surfaces into walls with thickness.

- add fillets (You can measure existing fillets to see .4mm) 

[johnwYMVVZ]

Thanks for the help!