Time-saving Tip for Re-using SolidWorks Drawings

by Josh on September 7, 2007 · Comments

solidworks tipsIf you feel frustrated each time you have to re-create a drawing, you’re not alone. All of a sudden, five other configurations and five other drawings are needed, all the same. Typically, you may open the part, start a new drawing, rinse, repeat. But, with just a few steps, you can save tons of time and get the drawings done quickly.

Where do I start?
So, you need to create five other drawings of similar parts that already exist. Say you have a bracket with a drawing, like the one below.

solidworks-bracket-drawing.jpg

There are five other similar brackets you need to detail. Here’s how to do it.

  1. Open the original drawing
    This will be the drawing that has the original bracket. Make sure the bracket is fully dimensioned and you have all the views you need.
  2. Save As… a new drawing
    Save the drawing with a new name to the location where you need it.
  3. Close the drawing
    Close down the drawing after you have saved it.
  4. Open the drawing
    Here’s the trick. Go to File, Open…, but before you actually open it, select References… down by all the check boxes.
  5. Replace the reference
    Double-click on the original part that is shown, then select the other part you need to detail. Hit Open, then OK and open up the drawing.

You should see your part change and you may need to move some dimensions, but you just saved a load of time by not re-creating the drawing all over again and again. Save your drawing and do it the same for the others.

Other Applications
You can also do this if you need to add more parts on a single drawing. After you do the above process, select all the views of the new part, Copy (Ctrl-C) them, create a new sheet in your original drawing and Paste (Ctrl-V) the views to get them on the sheet. You can also use this for more complicated parts and assemblies. This reinforces how important it is to use a standard method of creating parts, assemblies and drawings.

solidworks-bracket-model.jpg

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  • This truly is a great tip. I've been using this for the past year or so and it REALLY saves a TON of time.

    Also, another way to save time is to not have to create multiple drawings in the first place. You can accomplish this through a creative part-numbering system.

    For example, we'll design an extrusion that has multiple cut lengths. The main part number is 7 digits, following by a generic .XXX extension (I know what you're thinking. This wasn't my idea). The actual cut length has the full 10 digit numbering. So the Drawing Model are in the format 1234567.XXX For the model, you simply create multiple configurations. For the drawing, since the document is named 1234567.XXX, you simply show ONE part with all the views you need, and create a table to show the various configurations. For the extrusions, you're simply listing in one column the different cut lengths, and in the drawing the dimension that varies is labeled DIM "A". Each cut length will have a unique part number 1234567.006, 1234567.015, 1234567.024, etc.
  • That is a great tip too Bruce! Makes it very easy to add additional configurations.
  • Russell
    I use both configurations and this trick, depending on the situation.

    Configurations of views can be changed with a right click.
  • Great point Russell. Make a new config, copy views to a new sheet, and change the configurations. It's really that easy.
  • Hi Josh-

    Here's another drawing tip. How many times have you heard this: Make a new drawing of this new Bracket B just like this old drawing of Bracket A (Brackets A Bracket have completely different shapes)use all the same notes(lots of notes), revison block, title block...etc.

    Here's what I do; I Open the old drawing of Bracket A, then, I Save The Sheet Format; with the name Format Bracket A. Now, this Sheet Format will have all the Notes, Title Block, Revision Block, Annotations, etc.

    I Open a New Drawing, Insert the Views of Bracket B, Edit the Sheet Format, Window Select and Delete the Title Block, Border, Revison Block, etc. Next, RMB the Sheet Properties and Select the Sheet Format A. And there you have it. All the desire Notes and Annotations from the old drawing are now in the new drawing.

    Cheers,
    Devon
  • That's a great tip Devon. Seems like I always have to do that on large drawings to get the notes and stuff out of them. This would save time for sure. Thanks!
  • Josh,

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    Thanks,

    Mike email mike@accuframesystem.com
  • Jason
    Josh,

    That is a good tip! I've wanted for years to have a drawing open different models than the one it currently opens but didn't relize I could change the references when opening. I've always just temporarily renamed the files the drawing references so when it says it can't find them, I point it to the files I want it too. Then I make sure to undo my renaming of the files once my new drawing is saved with reference to the other files. But your trick works much better. Thanks!


    Devon,

    I'm curios why you said you have to edit the sheet format and window select to delete all of your title block, border, revision block, etc. You shouldn't have to do this. If you just RMB to Sheet Properties and select your desired sheet format, it removes the old sheet format for you. This should save you a step.

    Jason
  • Jason, thanks. Just wanted to mention also that you can do the same thing with assemblies before opening them up. Makes it really quick to replace parts.
  • Jason-

    RE:"If you just RMB to Sheet Properties and select your desired sheet format, it removes the old sheet format for you. This should save you a step."

    Yep, thanks for the correction. Sometimes, my brain thinks faster than I type.

    Devon
  • Chris Chastine
    Josh,
    I really appreciate this tip. I used to use SW Explorer to replace parts within my drawings but since 2007 came out there have been issues with that process. I just used your tip and it worked wonders.
    Kudos to you and thanks for all your tricks.
  • Chris, awesome. I'm glad it worked well for you. Thanks!
  • Jim M
    This is a good tip. I have used this before but forgot how to find the place to change the references. Thanks!
  • Hey Jim, glad the tip helped!
  • tom ruggiero
    Thanks for the tip, I've been using it a lot. I do have one problem. This does not work on assy. drawings...multible parts mating together. Is there a tip.
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