base sketch for multiple parts

[mmolt]

Hello all...

Question for ya.

My company uses a lot of extruded aluminum parts, and we often use the same base aluminum extrusion for different parts. So here is my dilema...

I want to have a base part which consists of a sketch that controls the cross sectional shape of the extrusion. Next I want to be able to use that base part in another part and use the extrude feature in Solidworks to create a part with some length. Next I might as some cuts, holes, etc. to the part.

Now say we decide we need to alter the base part sketch, I would need this change in the base part to change the other parts it is used in.

What is the best procedure to do this?

Thanks in Advance

-Mike

 

[ctopher]

Sounds to me the best use of a design table. Maybe dash numbers for each configuration which have certain dim's and extruded lengths.

 

[SBaugh]

Your trying to use a part time and time again, but not make any changes to the original sketch. Until you need too.

If you have Multiple differnt types of configurations of the same part then a DT will work for you, but if you start getting alot of different configs. The part will get so large and the MB will grow in size. The rebuild time for your assemblies could slow down in the process. But a DT or just making new & different configs is about the only choice you have.

My first suggestion would have been a library feature, but if you expect to change the default or original sketch and it affect all parts. Then a single part with a DT is the way to go.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

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[Heckler]

Mike,

This could be a configuration nighmare if not managed correctly. First, I think Scott is correct regarding make this a library feature. If you add features to the base extrusion it is considered IMO a different part and requires a unique part number. I can think of one situation where you would detail all parts on one drawing that would be a weldment. Just think about how you will manage this data and how it fits into you current data managment scheme.

 

[drawoh]

mmolt,

You can create your extrusion as a part, and load it into an assembly model. Attach your machining drawing to the assembly model. This works way better if all your extrusions are approximately the same length, although you can tabulate the extrusion to get varying length.

If your extrusion is custom, this conforms to a logical drawing structure. You need an extrusion drawing. Your machining drawing must call up the extrusion as a part.

JHG

 

[krywarick6]

How about a different way to skin the cat? It's long so bear with me.

1. Start a new part - 1 sketch for the extrusion base shape. Close the sketch and save the part.

2. Start a new assembly - insert the base shape part with the single sketch.

3. Set the View setting to view sketches, create another part, this time in context, build the base extrude and save.

This part is akward to use but if multiple parts are started this way, they are ultimately controlled by one base sketch and can also be used independantly - to an extent.

There is a bit to be desired with this method, but it could be another possiblity.

Regards,

Christopher Zona
Litens Automotive Partnership
Concord, Ontario, Canada

 

[MElam]

Here's another option:

1. Create the sketch, and either make a tiny extrusion or a surface fill. Save the part.

2. Start a new part. Go to Insert, Part... and select the part created in step 1 (if you used surface fill, check the box to bring in surfaces). This will make a "Derived part"

3. Select the face of the derived part and Convert entities, then extrude.

The derived part can be re-used many times, and any change to it will update the other parts