July, 2012 | CADD Edge Blog - Featuring SolidWorks 3D CAD Design Software

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How to Create Multi-Sheet Drawings With Different Formats

  
  
  
  
  

Jon S.  answers a common question how to handle drawings where the first sheet should be formatted differently than subsequent ones in SolidWorks.

One of the fun questions we encounter in Tech Support concerns multi-sheet drawings. If drawing template 1 has Sheet 1 set to come up with Sheet Format 1, how can we make Sheet 2 come up with Sheet Format 2 without having to browse to it?


Normally, when you create a second sheet, you are prompted to choose a sheet format size for this sheet. This can be difficult in large companies that have sheet formats stored in various locations or that must follow a certain protocol as to what the second sheet contains or follows. Originally, I looked online for a solution. I had noticed there was a posting on a blog about switching sheet format file names and trying to trick the program into accomplishing this task. But the steps were difficult to follow and no clear explanation was given.
In this post, I will show the quick way to accomplish sheet 1 with sheet format 1 and sheet 2 with sheet format 2. I will also show you a back door way.

Quick, Painless, Easy

Step 1) Create a drawing with your preferred sheet format for sheet 1. This example uses an A size Landscape.

SolidWorks Drawing Format Selection

Step 2) Add a second sheet with your preferred sheet format. This example uses an A1 (ANSI) Landscape.

Drawing Sheet Two Selection

Step 3) Go to Options> System Options> Drawings. Clear the check-box for “Show sheet format dialog on add new sheet.

SolidWorks System Options

 

 

 

 

 

 

 

 

 

 

 

Step 4) Save your drawing as a template.

Now when you create a drawing using this template, sheet 1 will have the main title block data, revision blocks, tables, etc. . . Sheet 2 will have the second sheet format and any other sheet after that will follow Sheet 2’s format.

 

 

Back Door Way

Step 1) Create a drawing. On this drawing, edit the sheet format to contain only the information needed on your second sheet of your template. Use File> Save Sheet Format to save this sheet format out.

Edit Sheet FormatSolidWorks Drawing Title Block


 

 

 

 

 

 

 

 

Step 2) Edit the sheet. Add any revision blocks, title blocks, tables, etc. that you require on Cover Sheetyour first sheet.

 

 

 

 

 

 

Sheet Properties

 

 

 

 

 

 

 

Step 3) Right Mouse click on the sheet and choose Properties. Set the sheet format to your custom format.

 

 

 

 

 

 

 

 

Step 4) Use File> Save As> .DRWDOT to save out your template.SolidWorks Drawing

 

Now create a drawing using this new template. Sheet one will have all the title blocks and tables on it. When you add a new sheet, it will use the exact same sheet format but without the extra blocks. This is because both sheets use the same format. The title block and tables are stored in the template data and not the sheet data.


Using SolidWorks for Construction Projects

  
  
  
  
  

Leon sent over this writeup of a building project he designed using SolidWorks.  I'm not sure how many decks have been designed using SolidWorks but the number has to be pretty high.

Did you ever have a weekend project that you needed to design and get your material lists?
I just had a friend ask me to build her a storage area in her condo.  I  immediately thought it’s on a 4th floor, so I need to get everything cut accurately ahead of time and it’s also not going to be easy to carry materials in so size will matter.  I decided to use SolidWorks to get the design laid out to make sure she liked the idea and the price of materials met her budget.  I was able to send her an eDrawing  to review the design.
 blog const6Weldment design in SolidWorks
I started with a simple layout sketch to capture the room size.  This makes it easy to make adjustments to the design size.  Adding relations to this sketch makes all the additional features update with the change of one sketch.
 Layout sketch in SolidWorks
 
The Weldment feature in SolidWorks came in very handy to keep the bodies separate automatically and make cut lists easy.  I started by creating the frame layout and then patterned repetitive joists or studs to speed up the process. 

When there was a need for an existing piece not consistent with a pattern, I just used the Move/Copy bodies command.  This made it faster and helped keep accurate material counts.
   
When all was done I had all my materials pre-cut and just brought them in for the final assembly.
Notice the stairs.  It was critical that I could fit them in without going into the living space, but also get enough head height at the top with the angled ceiling.  Having SolidWorks saved me so much time vs hand calculations.  If you'd like to download the SolidWorks file and see how I approached this modeling task you can use this link.

Finished Project

-Leon

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