Skeleton Sketch as Envelope Part?

[Randy1111]

I've decided the best workflow routine for our company if we go with Solidworks will be using assemblies with all part sizes and configs controlled at the assembly level.

The prefered method for this is to use a skeleton sketch of planes, axes, points, etc and then creating all the parts "in context" constrained to the skeletons reference geometry. The skeleton sketch can then be completly controlled via a single design table.

That all makes perfect sense to me. But while researching I keep coming along suggestions to make the skeleton a part, and insert the part as an envelope instead of creating the sketch in the assembly. Various places mention this as the 'better' method, none explain why.

I dont see why this is a better alternative. Several times its been mentioned that this way its not included in bom's or mass property calculations. But reference geometry in a sketch in an assembly wouldnt be either, so i dont see an advantage.

I do see it as a disadvantage in the editing area. If its an assembly sketch, I can open the design table in the assembly, input all the changing variables, and see the assembly update.
If the skeleton is an inserted part, i need to open the part, open its design table, update the part, then update the assembly. That just seems more ackward to me.

I must be missing something. Can someone explain any advantages/disadvantages to either way? I'd hate to get my company going one direction with new software then have to change it 6 months down the line because my workflow wasnt optimum.

Thanks in advance !

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Randy

 

[ctopher]

I personaly do not like in-context only because not a lot of users understand it and can screw up an assy. If I know I will be the only user EVER for that assy, then I will do it. Approx 98% of my designs are all separate parts inserted into an assy, then parts can be revised within an assy thru "edit part".
Also, separate parts can be used on other projects without the sometimes headaches of worrying about updating the assy the part was created by in-context.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-05)

 

[Heckler]

Nothing wrong with the Top Down approach as long as the entire design team understands it and your business processes follow that approach.

If the designs are unique in nature and the parts will not be used or modified for other products then Top Down works. We have found that our process drives us to use and reuse parts and "in-context" issues can waste a lot of design time. With that said, I also like the "no external references" option when doing Top Down modeling. That is a powerful tool.

I would do some more searching on Top Down & Bottom Up approaches to modeling before you get started using SWx.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[TheTick]

Envelope basphemy...

Putting master geometry at assembly level works fine. You just can't create surfaces or solids at the assembly level.

I designed hinges on my last job. I used a top-down approach similar to what you describe. A couple master sketches at the assembly level to drive the main part geometry.

Usually there was a base (static) leaf and a moving leaf. I would design the moving leaf in a fixed position as an envelope part. Then I would add the same moving leaf part (same file) as a regular part, which would be mated to the envelope. This allowed me to design the leaf in a fixed position and still have it as a moveable component without boogering up the features.

Don't use assembly level sketches to create part-level features directly. Copy assembly-level sketches to part-level sketches first (using "Convert entities"). Usually my first step in laying out a part from a master assembly is to copy in the necessary portions of the assembly-level geometry to the part.

Various places mention this as the 'better' method, none explain why.

{sarcasm}It just is. Ask anyone. Ask my mom. She'll tell you. Everyone knows that. GAWD!{/sarcasm}

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[Heckler]

Process planning is one of several major issues in product development. Top-down design and configuration tools help bring simplicity to the inherently complex endeavor of assembly modeling. Like Tick stated Don't use assembly level sketches to create part level geometry.....the "no external references" will help you keep the feature references at the part level.

Check the date on this link: It's about time and I hope SWx harnesses these types of methods

http://www.synthx.com/tom/sy_tip_9808.htm

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[Randy1111]

I was planning on creating the reference geometry of planes and axis's as a skeleton sketch within the main assembly. Then with each part, create matching reference planes, and constrain the parts planes to the assembly skeleton planes. Then constrain the part geometry to the part level reference geometry within its own file.

So your saying that is the wrong approach?
Convert assembly sketch to a part level sketch, then use that to drive the part dimensions?

I dont understand the "no external references" part. I'll have to research that some more. I have done quite a bit of research on the whole top down modeling within solidworks. Thats how I came to the conclusion that using the skeleton sketch was the most functional way.

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Randy

 

[TheTick]

Your approach is similar to mine.

As far as external references go, there's some debate. Usually it is best to eliminate them at some point. I keep external references "live" until a part is released into PDM for production. Then I eliminate them so all parts are self-contained. Usually I have a copy of my development model in the project archive.

 

[Randy1111]

Ahh I see now what your saying, once at final geometry, break the links, and then send the drawings to the shop, so someone doesnt inadvertently screw everything up. I can see that working well for us also.

My main purpose for the orignal file, all linked, is to create it as a template file. So when a new job comes in, we copy the whole folder, rename, change the assembly level design table. And were done. Break the links, print the drawings, and go on to the next project.



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Randy

 

[Regg]

Randy1111,

If your product is going to be done in one assembly, then making the sketch in the assembly is the way to go. However, in my business, our product is issued in many sub-assemblies. The skeleton sketch is put in each of these sub-assemblies. The advantage of using an evelope is that, when used in an upper level asembly, the envelope is not shown. I know you can hide the sketch but this way it is automatic. The other reason to use an envelope was that before the "Exclude from BOM" feature was added, the only way to exclude a part was as an envelope (without hand modifying the BOM).

Regards,

Regg

 

[AnnaWood]

Take a look at Sketch Blocks. This is fairly new to SolidWorks and allows for skeleton type modeling.

http://www.solidprofessor.com/flash/2006_Update_samples/Blocks.html

Regards,

Anna Wood

http://www.auerprecision.com

 

[AnnaWood]

Here is another link from the SolidWorks website for Sketch Blocks which are new in SW2006.

http://www.solidworks.com/pages/products/SolidWorks_2006/documents/sketchblocks.wmv

Regards,

Anna Wood

http://www.auerprecision.com

 

[Randy1111]

Those sketch blocks are interesting, now I have another item to research lol.

Regg, thanks for the info. Thats exactly what I was looking for. Our assemblies are single level, no sub assemblies, and less than 20 parts total. Very basic.

Several of the parts are purchased, with set sizes so will be made as configurations of a single part file. The majority of the parts, although always having a similar shape and layout, are rarely if ever the same size as a previous order. So thats why im looking at going the 'sketch template', copy and easily edit route.

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Randy