I have tried various methods to create a title block of my own in solid works and have not had very good luck. My goal is to use existing cad title blocks and insert them into the solidworks title block section. I have no use for the default title blocks that come with solidworks. Any advice on this subject would be greatly appreciated. gaitano
Gaitano,
I recommend just creating a new title block natively within SolidWorks. Then, save as Sheet Format under the File pulldown menu. This will allow you to insert it into any existing drawings easily, and also can be set up as your default within your templates. Remember, drawing templates and sheet formats are different. Templates can (and should) use sheet formats, but they also hold settings and custom properties. Look up both Drawing Templats and Sheet Formats within the SolidWorks Help for more details and the steps involved.
Matt
SW doesn't hold you to using their title block. One of the first tasks to undertake when working with SW is to setup your company's title block. You can work off the existing title block or off a fresh start. Either way you will probably want your imported title block to include SW functionality like using custom properties to fill in document values like drawn by, title, part number, etc. Once you have created a title block for the sheet size of interest you save it to a sheet format file (.slddrt) and possibly to a template file (.drwdot). The former allows applying the sheet format to any existing drawing and the second allows setting up all the other things your drawing must have to meet your standards.
Title blocks can be imported to a sheet format from dwg/dxf files also. They will likely entail some cleanup. Once cleaned up the methods from the previous paragraph apply.
TOP
I know how to make it from Acad dwg.
OK, let us suppose you have the title block in dwg format (With not exploded text)
You made that dwg in scale with a certain standard format. In Solidworks go, File > Open > select dwg Select your title block file. In the dxf/dwg dialog select
- Create new Solidworks drawing
- Convert to Solidworks entities Click Next Select
- Layers selected for sheet format Select all layers that form your title block Click Next Choose paper size that fits yours Center the drawing (if you haven't moved exactly your lower left corner of dwg sheet to 0,0 in Autocad or similar) Click Finish Now, right mouse click on drawing empty paper and select Edit sheet format. You can choose font and size of text. You can link any part of text of your title block to custom property (drawing or part) After you finish, select File > Save sheet format And you are done
Hope it helped.
Oz
It's best to create it natively from within SolidWorks though, yooz. Much cleaner processes, and some would argue it is more reliable.
Matt Lorono
I agree, blocks and border should be created in SW, yes its a pain to redraw and recreate but use notepad and copy and paste your text notes if there are a lot. I tried to do a "quick" import of all our blocks and border and SW 'seemed' to have taken it well, until I started using the template and then the problems started. Blocks doing crazy things like disappearing, leaders jumping all over, text styles not native to SW, imported, but don't print. And exporting back to autocad really causes everything to go crazy. Don't do it.
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