Hi,
I am trying to think how in SolidWorks, I would create an object to “wrap around” another.
Let’s make a concrete example to explain what I’m saying. If I have to draw a phone will there
be a quick way to use SolidWorks in order to automatically construct the case?
The object in question is not exactly a phone but it was the easiest way to describe my problem . I am working on an object for lost wax casting.
Thanks!
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You can use the intersect command, create the shape of the case in a box and then put the phone where you want (separate bodies) then you can use intersect to get rid of both the phone piece and the case piece by excluding features in the intersect (it gets rid of them). You might want to scale the phone (or other object) slightly so that you don’t end up with a case that has no tolerance and won’t fit.
You can try subtracting bodies. Create two independent bodies in Solidworks, then use the “Combine” feature to subtract one body from the other.
In your example, you can create the design for the case by building it around the phone model without worrying about the interface. When you’ve finished your design, you can subtract the phone’s form from your design area to create the interface with the phone. If you’re looking to 3D print it, then you might want to offset that interface a little as well so the phone fits.
Hi,
I have recently made this but I can’t describe exact buttons to use because I’m rendering animation and it might take some time.
This is what I did:
- I made assembly with solid part (1)(outside shape only) and another part (2) which I want to cut out of solid.
- By editing solid part(1) in assembly I cut out part 2 (this is the button I don’t know exactly).
If you still don’t know how to do it later today I can tell you exact process.
Sorry I can’t help you more right now.
Jan
I also agree with using intersect. There’s a slightly different way to make something like a phone case as well. You can use the Surface Offset command which will take the selected faces and move them a desired distance away from the selected faces. These can then be made solid using the Thicken command.
There are difference ways to do this, I will show the 2 easiest methods for you:
1. If you don’t already have a case designed:
- Save the phone design and start a new part (or assembly, personally I prefer to use it in part mode).
- Go to Insert/Parts and choose the phone file.
- Use the Shell function: This function give you 3 difference thickness:
Zero: for places that you don’t want to cover (screen, buttons, and so on). Select the faces in the 1st box, use preview mode as Solidworks does not always able to make zero where you want.
1st thickness: Entered in the first box, then select preview and shell outward to make it outside of the part.
2nd thickness: check multiple thickness to use. It/they are the surfaces you want to have difference thickness than 1st.
- If Solidworks fail to make preview go back and deselect the surface(s) or change thickness.
- Now that you have a shell, add extra design/cosmetics that you want. Maybe cut out the buttons or ports that the shell function does not accept.
2. If the case is already designed:
- Save both files and start a new part/assembly.
- Insert both and use mates to arrange them if necessary.
- Use Combine function and choose Subtract mode, use teh case as base object and the phone as to remove.
- Cut out holes for screen, buttons, ports if necessary.
P/S: Shell works best if it is Solidworks parts, import parts may need to be convert to solid and/or recognize features.
2 Likes
You can try inserting the phone geometry into a solid block using assembly. Then edit the block in the assembly and select cavity and click on the phone geometry. Using then using a combination of the surface offest and split command you can have you inner phone geometry with a flat outer surface.
Hello Mr. Amirfar,
One approach is to build a body at the parting line around the phone or let’s say in the mobile phone situation. the top face of the phone. and use boolean/multi body operation to carve the cavity of your mobile.then you will be having back case surface. which you can scale it to larger size so that it can fit when 3d printed.
Not a bad way to do it, but rather than subtract, use the Indent tool. This gives you more options for following the contour of the part.
Another option would be to simply offset all the surfaces that make up the face you want the case to cover. Then, you can thicken the surface to the desired thickness you want to use.
Indent is indeed the easiest in this case, as you can define the air-gap between the ‘phone’ and the ‘case’ in the same feature.
Hi,
The indent tool is perfect for this as most often you want to control the clearance between the two parts.
Say 0.3mm for 3D printing and 0.1mm for injection molding, to take into account distortions, shrinkage and tolerances.
Alternatively use the offset tool which you can then thicken and if the thicken feature does not work, it’s a matter of reworking the surfaces until it does.
When in the end Thicken fails, I offset the initial surface to the inner and outer depth of the new intended part and then connect the two offsets using newly constructed surfaces, often Boundary surfaces, then you knit them together in the end to form a solid. It can be a tedious part of the job.
A simplistic but quick way would be to scale up the initial object to the target distance of the inner and outer surface, then boolean the inside away.
First create the general shape then use the shell command to make it hollow.
one thing you will need to consider is the amount the material will shrink when you cast it you will need to scale everything up in order to account for this.
hope this helps
