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more than 1 part per drawing

usually, well since i started using SWX, i have always had 1 part file per drawing file, with multi drawing files for parts, assy's and bills. now i have a customer that wants as many parts per a sheet as i can fit on there. my templates are such that they utilize props as much as possible. how should i go about getting multi parts onto a single drawing and still have the props perform correctly? (first on dropped on populates the title block) is there a way to create the typical det no., description/name, heat treat, req'd, etc. under each part model and have it pull from the part props? i had to go back and combine a recent job i was already finished with and IT WAS A PITA! any help is hugely appreciated. THANKS!

Reply to
3d
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"> usually, well since i started using SWX, i have always had 1 part file

I don't use the properties to populate the title block. I often put multiple parts on one sheet. I can populate notes with properties for each part on the sheet. There is a spin box when designating the property to choose the prop associated with the part in the selected drawing view. I also do most of thisd manually, so my input may not be valuable to you.

You will probably need to create a special template just for this sort of thing.

Good Luck.

jk

Reply to
jk

Create a block with the string text for the properties. I have used this method before and it worked quite well. However I believe it was in SWX 2004. I have since not had the need for multiple details per sheet.

mrcswp

Reply to
mrcswp

BY ATTACHING THE BLOCK TO THE VIEW IT WILL PICK UP THE PROPS FOR THAT MODEL?

Reply to
3d

There is definitely a way to extract properties from the associated drawing view. Its been a while since I had to configure this, but I simply copy a block of notes with property references, select the proper drawing view by clicking on it, and then paste the block of notes. I do have to manually move the notes to the proper location, but everything else is correct and they update dynamically.

If you need some detail about the configuration of the property references, I can look through some old entries and provide a description.

Reply to
John Eric Voltin

There are two ways we do this:

  • We put a (sub-)assembly on the drawing, add a complete BOM on the drawing. Then we put (a few of) the parts of this assy in separate drawing views. The you also can add balloons (connected to the assy) next to the parts. With the "more properties" of these balloons you can remove the connecting lines. The Title block of your drawing will be filled by the properties of the assembly (depending on your template).

  • You also can put muliple parts/drawing views on your drawing and then separate BOM's for each part/drawing view on your drawing next to the part. In each BOM you recal the recommended properties. When adding these BOM's, remove the Tick from "Attach to anchor". The Title Block of your drawing has to be filled manually.

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"John Eric Voltin":

Reply to
\/\/im

Yes. Create a block with the note references, then insert the block on the view you want to extract the data from.

Reply to
mrcswp

Here, we put multiple parts & assy's on a sheet. The title block is manually controlled by custom properties that are accessed from the File/Properties/Custom area. We have multiple BOM's on the sheet as needed, and with the new SW BOM, have started using the functionality of putting more than one config in the BOM if we have something like a LH & a RH that have unique wlmts, or something.

WT

Reply to
Wayne Tiffany

There are two ways we do this:

  • We put a (sub-)assembly on the drawing, add a complete BOM on the drawing. Then we put (a few of) the parts of this assy in separate drawing views. The you also can add balloons (connected to the assy) next to the parts. With the "more properties" of these balloons you can remove the connecting lines. The Title block of your drawing will be filled by the properties of the assembly (depending on your template).

  • You also can put muliple parts/drawing views on your drawing and then separate BOM's for each part/drawing view on your drawing next to the part. In each BOM you recal the recommended properties. When adding these BOM's, remove the Tick from "Attach to anchor". The Title Block of your drawing has to be filled manually.

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Reply to
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