Break association of drawing with model

[slorandy]

I would like to use a SolidWorks model to put a Model View in the drawing for another part as a reference image, and then unlink it from the model. I'm creating drawings where I want to show what the mating part will look like but I don't want to provide the model. Is this possible?

 

[charbroil]

This sounds like a good application for an Alternate Position view if I'm reading you right.

If you have a configuration in your assembly with the mating part shown, you're ready to go.

In the drawing, activate the view you want to show the part referenced in and choose the Alt Position icon (1 vertical bar and 2 horizontal ones with squares on the ends).
Choose the "Existing Configuration" radio button and pick a config with the mating part visible. Hit okay.

Your mating part will be in the view, but in faint phantom lines.

It's a very cool and handy command. I hope that's what you were looking for.

System: Dell Precision 650—Intel Xeo @ 2.66 GHz with 1/2G RAM
OS: Windows 2000 SP3
Graphics: NVidia Quadro FX 500 128Mb (OpenGL set to Solidworks)
Version: Solidworks 2005, SP0.1

 

[TateJ]

Another interpretation of what you want...
If all you want is an "image" of the part - then just drop an image into your drawing. SolidWorks is OLE compatible - means you can copy/paste a BMP or JPG into your drawing. Will that get what you want?

tatej usfilter.com​

 

[MadMango]

Wouldn't Isert Named View work just as well?

[green]"But what... is it good for?"[/green]
Engineer at the Advanced Computing Systems Division of IBM, 1968, commenting on the microchip.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[slorandy]

TateJ: I think using the word "image" was misleading.

Hopefully this will clarify. I'm working on the drawing for Part A (not an Assembly) and want to insert a Isometric View of Part B (for reference only) but then not worry if the Part B Model is deleted or placed in a different location on the network.

 

[TateJ]

OK - if you worry that the part you want to "reference" will be deleted - make yourself a copy of it. If it gets moved - SolidWorks will ask you to find it again. I'd go ahead & insert it as a model view, if it gets moved - worry about that later. Make sure it won't get deleted, though.

BTW - would this be better as a drawing of an assembly with an exploded view - rather than a drawing of a part?

tatej usfilter.com​

 

[slorandy]

I understand how to do this if the model of Part B is available. I want to know if there's a way to break that association and loose the model view.

 

[J-C]

Create a new drawing with the view you want. Translate the view out to dwg and then import it back in (Comes in as as sketch items).

In your main drawing, create an "Empty View" then cut and paste the dwg sketch geometry into that empty view. The empty view makes it easier to move around, scale, etc.

Jason Capriotti
Smith & Nephew, Inc.

 

[macPT]

One of the key feature of SW is that drawings/assemblies are allways updated. If you modify Part B, in the case that you broken the link of drawing part A, this drawing will be outdated. Even if the Part B view is just for reference, you have the risk of having erroneous information in an approved drawing.

If your problem is the possibility of change the location of part B, then this is a false problem. Why? To be productive and to have quality assurance in your design (example, document control) you must have a well known folder structure and well known rules to save and transfer your documents in this structure. Part B cannot stay anywhere else. In Options, tell SW where to look for files in this folder structure (otherwise, refer to TateJ's last post).

Regards

 

[slorandy]

Gildashard, how do I "Translate the view out to dwg"?

 

[charbroil]

macPT: If you modify Part B, in the case that you broken the link of drawing part A, this drawing will be outdated. Even if the Part B view is just for reference, you have the risk of having erroneous information in an approved drawing

Very good point here. If that component changes even the slightest bit, you'll have people questioning you on it, guaranteed.

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slorandy, you could also do the following: Have the SW Model file open of the component you want to reference.
Save As... a JPG picture.
Read that picture into a photo editing software.
Draw a box/mask/marquee around the area you want your picture to be.
Use the CUT function (usually CTRL-X).
Go back to that SW drawing of the assembly.
Paste the clipboard contents (CTRL-V).
Now you've got an unassociated, resizable picture of your model in the SLDDRW document.

This is a variation on the oldschool printscreen method from when printers hated my CAD/CAM software. Microsoft Paint became my best friend.

System: Dell Precision 650—Intel Xeo @ 2.66 GHz with 1/2G RAM
OS: Windows 2000 SP3
Graphics: NVidia Quadro FX 500 128Mb (OpenGL set to Solidworks)
Version: Solidworks 2005, SP0.1

 

[charbroil]

…and TateJ mentioned the same method earlier, too.

System: Dell Precision 650—Intel Xeo @ 2.66 GHz with 1/2G RAM
OS: Windows 2000 SP3
Graphics: NVidia Quadro FX 500 128Mb (OpenGL set to Solidworks)
Version: Solidworks 2005, SP0.1

 

[jhricm]

Create the drawing and save as a .dwg. Open it cut and paste into new drawing. Then make this into a block so that you can position it. Complete the rest of your drawing.