How to create housing around an existing part ?

[cyucelEJ2QP]

Can you please give me some pointers if what I am looking for is possible in Fusion 360 ? It is hard to describe, otherwise I'd expect my google queries to return something sensible, sorry ...

Attached is a design with a Micro Servo and just below it a rectangular box.

What I would like to do is somehow either extrude box further to the top of the servo, or push the servo into the box so that it ends up in a housing with a tolerance of T. 

My first inclination was to project servos profile and do an extrude cut, however this only maintains the parts shape in one plane and the bottom would be a flat surface instead of creating a contour below part's bottom details.

Hope this is making sense, basically, the box is a plastic piece and I'd like to make a housing for servo to pushed into to keep it in the correct location, while the end is extruding from the side of the box. Needless to say the bottom of the box is to be shelled.

Many thanks

[davebYYPCU]

I can’t open your file for some time yet.

Same process if adding material to top of servo, using outside of sketch detail, or removing material, pushing servo in, uses inside the sketch detail.

Use your idea, but with 2 Extrudes.  Std Extrude Cut the servo (socket) outline, pocket depth, (or to object if required) as suggested yourself.  

Second Extrude, is Thin Wall, Cut with T wall thickness (from same sketch), depth same as the socket.

No idea what you mean about bottom contour.

Might help...

[cyucelEJ2QP]

Thanks @davebYYPCU , perhaps bottom contour wasn't the best description. What I meant was, the bottom of the servo is not flat (it is sitting on its side on this occasion) - screen shot attached.

What I'd like to have is for the bottom of the housing to take the shape of the bottom of the servo. Instead of a flat surface where the servo sits on it's screw plate (similar to what's already on the screenshot).

[laughingcreek]

what are you considering the "top" of the servo.  in your file it looks like the box is off to the side of the servo, not below it.  sketching your intent on a screen shoot of the part would be helpful

[davebYYPCU]

Same thing, but with box for lugs done deeper. 4 Extrudes.  (Working side on for 2 Extrudes is simpler, centreline sketch, and symmetric for both Extrudes.)

Combine cut is just as fiddly, with press pull for tolerance, especially with that gearbox outline.

Might help....

[cyucelEJ2QP]

Hi @laughingcreek , attached is the (kind of) the end location for the servo, inside the box fully, but the servo head and the top partly on the outside. I can of course go ahead and use servo as a tool body and perform a cut, this leaves a perfect impression of the servo in the box but 1. I will not be able to slot the servo in from the top and 2. Cannot think of a practical way to establish tolerances for actual servo to fit in there when printed.

[davebYYPCU]

What part of Thin wall Extrude are you not understanding?

[TrippyLighting]

1. Do you understand the difference between a body and a component?

2. Are you familiar with Fusion 360 R.U.L.E #1 & #2 ?

[cyucelEJ2QP]

I think I failed to make the question clear enough. Let me try to rephrase:

How to create a recess (indent) into a solid body for all or most of an arbitrarily shaped part to be slotted in. The recess created is to be in the shape of the part it houses, with the exception of the sections directly above the part so that it can slot in. Imagine a complex-shaped battery fitting into the battery compartment of a device.

Sorry @davebYYPCU , watched a few Thin Extrude videos, not sure how they can help with this? I might be missing something obvious.

A potential workflow I came up with is:

1. Place the part in its desired location in the solid body.

2. Cut out using the part as a tool body.

3. Create a sketch on the top surface of the solid body and project the top cross-section of the part.

4. Extrude projection down, to the lowest point where it fits (there are cases this wouldn't work).

This works for my purpose. However, I couldn't find how to add a tolerance.

1. Is there a way to enlarge an arbitrarily shaped recess by x mm?

2. Or even better is there a way to make the part a bit bigger before step 1 of the workflow? Part comes via a STEP file and gets added to the design. Scaling it out slightly would help however fusion doesn't seem to allow scaling of the bodies that are added in this fashion. Furthermore, scaling out would provide a % increase in size while I need an absolute 0.2mm in all directions, regardless of the size of the part.

[laughingcreek · Accepted solution]

Before going further, is this getting closer to what you want?  Seems to be what your discribing, but I'm unsure why you aren't utilizing the mounting screws on the servo housing. file attached.

[davebYYPCU · Accepted solution]

There are many ways to do this process, 

initially I responded - “from where you are at now”

You said you had a top down sketch of the projected body.

so depending on overall project, how many servos are in the Project, likely to use the servo as a component with centreline sketches.

Insert the component to in place position.  

Combine Cut or Extrude Cut that servo from the surrounding material.  

Second step is to Thin Wall Cut the outline sketch of the body, setting Wall Thickness As your 0.2mm.  Set the cut to be outside side of the body profile.

So in the same process, you could skin the body with 0.2mm Tolerance As Join, and then save it as a cutter body to place in position, and Combine Cut the material as one step.

I fit servos in wing / fuse pockets, with servo covers as a daily routine.

can demo for you later tomorrow.

Might help.....

[etfrench]

---

@cyucelEJ2QP wrote:

I think I failed to make the question clear enough. Let me try to rephrase:

How to create a recess (indent) into a solid body for all or most of an arbitrarily shaped part to be slotted in. The recess created is to be in the shape of the part it houses, with the exception of the sections directly above the part so that it can slot in. Imagine a complex-shaped battery fitting into the battery compartment of a device.

Sorry @davebYYPCU , watched a few Thin Extrude videos, not sure how they can help with this? I might be missing something obvious.

A potential workflow I came up with is:

1. Place the part in its desired location in the solid body.

2. Cut out using the part as a tool body.

3. Create a sketch on the top surface of the solid body and project the top cross-section of the part.

4. Extrude projection down, to the lowest point where it fits (there are cases this wouldn't work).

This works for my purpose. However, I couldn't find how to add a tolerance.

1. Is there a way to enlarge an arbitrarily shaped recess by x mm?

2. Or even better is there a way to make the part a bit bigger before step 1 of the workflow? Part comes via a STEP file and gets added to the design. Scaling it out slightly would help however fusion doesn't seem to allow scaling of the bodies that are added in this fashion. Furthermore, scaling out would provide a % increase in size while I need an absolute 0.2mm in all directions, regardless of the size of the part.

---

Surface workspace: Offset Face can give you 0.2mm, but you may need to select multiple faces. 

Solid workspace: Shell can also create a 0.2mm increase in the entire body.

Sketch: The projected geometry can be offset 0.2mm.  You may be able to use Extrude/To Object in order to remove all of the material above the servo.

[Bunga777]

I assume that after cutting the part, I can just offset the required surfaces, but is that not acceptable?

I wasn't sure which direction to insert the part from, so I hollowed out the one with the mounting screws.

I understood that the intention was to offset it in this way.

Click here to see the video.

https://knowledge.autodesk.com/community/screencast/2b0c56e1-f4a1-489a-9b1d-9c5378b125e7

I have also attached the data for your reference.

[cyucelEJ2QP]

Thanks again all ! Here is the end result: