How to control scales when exporting DWG drawings?

In SW drawings I have set the critical views (such as the flat patterns) to the seet scale. When I export to DWG, the options shows
the correct scale, but the DWG drawings some times have weired scales, i.e. correct dimension text but incorrect scale.
What is the best way to control the scaling for exporting DWG drawings?
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SW drawings output 2D geometry (to dwg, dxf) at the same scale as the sheet/view. You do get a message telling you that the dims don't match the geometry. but that's about it.
The only way we've been able to make this work is to output from SW at 1:1. Luckily, it's not required very often.
Regards
Mark

to the seet scale. When I export to DWG, the options shows

i.e. correct dimension text but incorrect scale.

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I don't get any messages telling me that the dims don't match the geometry. Im using SW2004.

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You will get the message if you have two or more different scales. For example, you have views at half scale, and detail views or sections at full scale.
You will find that your .dwg file will have the views 1:2 and the details or sections at 1:1. This can be a very frustrating thing if you are doing multiple exports. You will produce a drawing that looks like your .SLDDRW, but it will be a mess. SolidWorks knew your main view was half scale and set DIMLFAC to .5. Your vector data for the views will be at half scale. Knowing this, you can drop and drag your standard layout(s)and dimstyle(s) into the .dwg.
Cut the 1:1 details, sections (and annotations and probably the titleblock) from model space and paste into the layout. Back in model space, scale the views including the dimensions 2X to make all the vector data 1:1. Set dimstyle to your standard. Update all your dimensions. Back in the layout you will need to click in the viewport and set it to .5XP or 1/2XP. Lastly, type DIMLFAC and type 1. All will be as you want. I hate having to do this when a vendor wants ACAD because his CAD is ACAD not SW. It's even more of a chore if you have a tabulated part and you used Excel to do the table (because it was easy to produce on the SW side. You will have to cut and paste them individually and reset the size.
Jeff
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when exporting (save as), select the options button in the save as dialog box and select 1:1
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I export flat patterns all the time so I can create my laser files for our sheet metal parts, and I used to run into the same problem all the time.
What I do is I have a drawing template file set up that is empty, no title block or border. I bring my flat pattern into that and insert it with a custom scale of 1:1. That way I always know it will be 1:1 when I export it out to a .DWG file. It's a little extra work, but at least now I know my flat patterns are always 1:1 when I export them. I was having to redo to many because of the problem you're having.
Richard

to the seet scale. When I export to DWG, the options shows

i.e. correct dimension text but incorrect scale.

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