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external reference help


sandeep410

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Suppose i am making a box and a lid to box.After i make both the part.How can a add refernce to lid such that if i change box dimensions lif dimensions should change automatically to fit properly.

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There are 3 (or 4) ways to do this.

1. Easiest - multi-body solids master in a single sldprt that you then push out to individual parts.

2. Assembly level in-context modeling. (top-down modeling)

3. Spreadsheet driven dimension parameters.

 

I think there are built-in Help tutorials that cover each of these. There are also combinations of these techniques.

Edited by JD Mather
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What are the problems with 1 and 3? 1 is the way i would model it and I feel the most stable.

 

2 is basically you model the lid once you have created the assembly with the box. This allows you to use Convert Entities in a sketch for your lid that will adjust if you ever change the box. To me this is an extra step thats not needed if you use multi-body solids. If you have a part with 2 solid bodies you simply have to right click on the solid body(in the feature tree solids folder) and "Add to New Part". You will end up with 3 files. The sldprt file with both bodies then a file for each body. These files would then(if you want) be placed into an assembly file. If you ever change the part file with both bodies, each part file with individual bodies and the assembly file will update.

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problem with 1st is it doesnt show in bill of materials.And i dont wana use design tables as our file names are referenced through SAP and hence it gets messed up since design table has only one file name with diff config

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With the parts i deal with(plastic housings) we create all pieces in one file then insert them into their own part files. So 5parts, 6 files. Each part file will have its own line on a BOM and all 5 parts can be editied In Context from the original part simply by right clicking on the part and chose Edit In Context. Its really an efficient way to do it. Especially when you are dealing with matching complex shapes or organic surfaces.

 

And the option for using spreadsheet driven parameters doesnt always mean the parts have to be in the same file. The excel sheet could be referenced in both files, but i dont think this way is best. JD's order would be mine as well with multi body.

 

 

If you want to pursue option 2 then you simply need your two part files in one assembly and make sure you have the External References button(next to edit component on your Features ribbon) to allow external references. If you are editing your lid you can apply sketch relations between your lid and box or you can simply Convert Entities on your box profile into your lid sketch. Basically you are drawing the two part files at the same time as opposed to separately in part files. The issues that arise with this type of modeling come from the relations and knowing exactly how they work.

 

 

I would at least give #1 a try with a simple example, split a multi-body solid(2 parts) into their own part files with a naming convention for your BOM and go from there.

 

For instance say if you were making Box i would call the multibody file Box1.0, then I would have Box_Base1.0 and Box_Lid1.0.

 

 

 

What version of SW are you using?

InContext.JPG

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