Part drawings varying based on assm configs 2

[oogabubchub]

Hi everyone
I've created a top-down assembly of a machine that varies in width. There is a 16", 20", 24", and 32" wide version of the machine. The width is controlled by a layout sketch with a dimension set by the Design Table/Configurations. Some of the sheet metal parts vary in width due to changing size of the assembly.

I need to create drawings for fabricators to bend these parts and need accurate dimensions. In order to do this, I created an external file from the virtual parts, then inserted them into the drawing. I can't seem to figure out how to make separate drawing files based on the various configurations of the parent assembly. All the drawing models seem to take on the dimensions of whatever configuration the assembly is currently in.

 

[drawoh]

oogabubchub,

That sounds just how SolidWorks ought to behave.

In SolidWorks, top down is an excellent design strategy, and an awful manufacturing strategy. Fabrication drawings that update themselves depending on what drawing and configuration you have open is a potential disaster. The basic rule of thumb is that every single thing with part number 12348 must function interchangeably with every other part. No changing widths.

At some point in your design process, you must freeze everything. Replace the in-context geometry with geometry controlled at the fabricated part level.

If you have an assembly with multiple widths, tabulate the assembly drawing and the affected fabrication drawings. Assembly 12345-32 will call up sheet metal 12348-32. Assembly 12345-24 will call up sheet metal 12348-26, etc. You have one assembly drawing, and one fabrication drawing.

JHG

 

[CorBlimeyLimey]

With all due respect to drawoh, there is no "must" about it. Many people state that it is good practice to break all references ... many people state the opposite. I use both methods depending on the product.

One way to do what you want is to create a separate set of part drawings for each config. When creating the drawings, make sure that every view references the correct config. (RMB the view > Properties > Select config)

 

[MadMango]

I do a mix. I break all in-context references (after the design is final) and create tabulated or individual drawings for Parts that have configs, based on complexity of the Part. Whatever method works for your organization and comfort level with SW should be used.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[NomLaser]

"Whatever method works for your organization and comfort level with SW should be used."

It will also depend on your past experiences with older versions and their lack of functionality.

I have been burned in the past by not breaking external links. I don't deny their role in speeding up the design side but the documentation and detail side it can be a killer.

 

[EEnd]

Try:
Make a configuration in each part file for each different size. The dimensions which change based on the assembly configuration will need to be set to vary by configuration.
Have the assembly select the appropriate part configurations in addition to the dimensions in the layout sketch.
Link the drawing views to specific configurations of the parts.

Eric

 

[EEnd]

The attached shows that you can do what you originally asked about. It contains an assembly, 3 part files and a drawing. The size of the parts are driven in context by a design table controlled sketch in the assembly. The drawing show the 3 differently sized configurations of each part.

I think the others have presented valid warnings on if you should do this.

Eric

 

[oogabubchub]

Thanks a lot for all the help The solutions make sense and I'll try them out.

 

[oogabubchub]

EEnd,
I checked out your file and that's exactly what I wanted to do. It took some tweaking, but I managed to get it working for my own situation. I don't know what specifically it is that I changed that made the difference, but whatever it is, it works now. Thanks