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mark-hale

Solidworks help

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Hi

I am trying to think how in solid works, I would create an object to "wrap around" another.

For example, if I were to draw a phone is there a quick way to make solid works construct the case?

The object in question is not as simple as a phone but figured that was the easiest way of explaining what I was trying to do. I am working on an object for lost wax casting.

Cheers

Mark

 

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You could try using an Indent perhaps? Draw your "case", position your "phone" inside the case. Choose the "case" as your target body and your "phone" as the tool body. Check the "Cut" option and specify a clearance.

 

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Similarly, you can use "Offset Surface" on all of the external surfaces, with a 0mm offset (Or whatever you want your gap to be), and then use "Thicken Surface" on that copied surface to create a solid shell around your object.

 

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I would follow a similar path to Nick;

- In the "phone" part, do an offset surface with either 0mm offset if you want a line-on-line base "hole", or an offset of your choosing if you want a gap.

- Create the general shape of the base that you want in a new part, then insert the "phone" part into the base part and mate accordingly.

- You can now use the offset surface in the "phone" part to cut away the material in the base part (Insert > Cut > With Surface)

 

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I am not sure exactly what you are doing, but it sounds like the SHELL feature would help, you can import an object, make a little flat spot and tell SW you want to make a shell of the solid piece, all you do is provide the shell thickness.

 

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Many dont know that SW can also boolean solid adds and subtracts. Also there are features in the plastics molding modules that may help. I would model the object you want to 'fit', modle the object to encompass the other and do a boolean subtract. I have done it a few tkmes, but not enough to explain it w/ o looking at the program. When i get back to the office, ill look into it and make a post.

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wow - many thanks everyone for the options, I think the Shell will do the trick, have just run a quick YouTube search and that looks like the one. Will also have a look at the others as certainly worth having multiple options.

That's the one great thing I like about solid works, a number of ways to solve a problem.

Mastory, your idea sounds interesting, would certainly appreciate knowing what that is all about if you have time.

Cheers everyone.

 

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Mark,

 

The process in SW2012 is something like this:

Starting from within an existing part file

Insert;

Part;

Select part file to insert. (make sure to check "Locate Part with move copy feature" at the bottom which allows a crude mating process to locate the inserted part to the other. With out this selected, there is little to no control over positioning.)

Next, Insert;

Features:

Combine; (select add or subtract as necessary)

Select "main body" (if subtracting, the one to subtract from)

Select "Bodies to combine" (bodies to subtract if subtracting)

Search Solidworks Combine Subtract on youtube. There should be a few videos to step you through it.

. The video shows adding, subtracting and intersecting bodies of the same part. I would suggest doing it by inserting one part into the other like above. Then you have 2 fully parametrized models that you can edit independently. Depending on your process the multi-body part may also have advantages.

Matt

 

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I am not sure exactly what you are doing, but it sounds like the SHELL feature would help, you can import an object, make a little flat spot and tell SW you want to make a shell of the solid piece, all you do is provide the shell thickness.

 

This one is close. Model your phone as a solid then convert to surfaces. Trim away everything you don't want as part of the case. You will now be left with a surface similar in shape to a flattened rectangular soap dish. Offset this surface outward by whatever thickness you want the case to have et voila.

 

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