How do I create a solidworks title block from a cad title block

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
http://sw.fcsuper.com
Co-moderator of http://groups.yahoo.com/group/solidworks/

 

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
http://sw.fcsuper.com

 

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.