SolidWorks drawings are made up of three pieces:
- Drawing Template
- Annotations/Model Views
I didn’t make a mistake. There are three pieces. The drawing template includes a sheet format – three pieces.
- Drawing Template
- Sheet Format
- Annotations/Model Views
All of those combine to make up a drawing - *.slddrw.
SolidWorks gave us a separate sheet format so we can have the best of both worlds – standardized drawings at the tip of our mouse, but also custom title blocks and borders to match our company requirements. To save a sheet format, when a drawing with the one we want is displayed go to File > Save Sheet Format.
Check out the blog post from last year - http://www.caddedge.com/blog/bid/151868/how-to-create-multi-sheet-drawings-with-different-formats
The sheet format (*.slddrt) contains the border, title block, sheet size, and some other items. Check out all of the stuff in the FeatureManager under the sheet format:
To better demonstrate, here’s a page from the Drawings training class:
The sheet format (*.slddrt) is part of a drawing template (*.drwdot), as I mentioned earlier.
Drawing templates contain all the document specific information that is found in the Tools > Options > Document Properties dialog (i.e. units, standard, fonts, arrow sizes, etc.).
Combining the slddrt and drwdot with a model view and/or annotations makes a drawing (*.slddrw)
Let’s dig a little deeper.
With no other files open in SolidWorks, start a new, blank drawing. See that dialog?
The browse button will tell you the location of the sheet format – the slddrt – used for each drawing - Tools->Options->File Locations->Sheet Formats.
So, when we tell SolidWorks to start a drawing, it goes where we tell it in the File Locations for Documents TEMPLATES (tools->options->system options tab->File Locations)
In this case, I have two locations specified in File Locations for Document Templates -
a TEMPLATES folder and a TUTORIAL folder – those correspond to the tabs in the above screenshot.
When I select “Drawing” in the above dialog, SolidWorks goes and gets the drawing template (*.drwdot – not *.slddrw) from that file location.
So, if I want to change the title block on all of my standard drawings, I can either change the sheet format or the drawing template, because the drawing template contains the sheet format. Alternatively, if I want to change the arrowheads or the drafting standard – ANSI, ISO, etc. – I have to change the drawing template.
I recommend working with drawing templates to set up reusable formats such as company standards. It’s simple – just get the drawing to look the way you want and save the template (File->SaveAs->Save As Type->Drawing Templates). Otherwise, it’s just as easy to save the whole drawing with empty or no views to use as a standard.
Sometimes it makes sense to save the sheet format for reuse. The best reason I can think of to save sheet formats is a need for different formats for sheet 2. But for most Customers, saving the whole drawing with empty or no views is the shortest path to "done".
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.
Step 2) Add a second sheet with your preferred sheet format. This example uses an A1 (ANSI) Landscape.
Step 3) Go to Options> System Options> Drawings. Clear the check-box for “Show sheet format dialog on add new sheet.”
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.
Step 2) Edit the sheet. Add any revision blocks, title blocks, tables, etc. that you require on your first sheet.
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.
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.
Can you make an image like this in a SolidWorks drawing?
Sure you can. All you have to do is:
- Open your assembly.
- Make a configuration.
- Create an assembly feature that cuts away the outer casing.
- Make a drawing of that configuration.
- Apply the hatching as a drawing feature.
While you were doing that I added shadows to mine.
How about adding a parts list that cross highlites to the geometry and can be viewed in a web browser? Like this one.
If you are browsing with Firefox you can view an interactive version of the file. I don't have the web skills to make it work on other browsers, but since I can view the SVG file in IE I can't imagine its that hard to do.
I made these images while preparing a webinar we just ran on the new features in 3DVIA Composer V6R2012, the latest release that came out this summer. This release now support the multiple section planes that I used in the earlier images. Prior to that I could only have one section plane in an SVG image. These views are great for service manuals, product documentation, or spare parts catalogs. And best of all the tool is designed for anyone to use. You don't have to be a SolidWorks user, so you can let the person who needs the image create it based upon your designs instead of creating it for them.
If you missed the webcast we'll be doing it again so keep an eye on the schedule.
I just saw that SolidWorks 2011 SP3 is now released and available for download. I like to skim through the release notes and see if there have been any enhancements to the software. Often they will sneak things into service packs with little fanfare.
In this case I saw this item: "Ability to disable the drag annotation “combine/snap” in drawings." SolidWorks 2010 added a great feature where you can drag a note onto a dimension or another note and it would merge them together. This can be very handy building numbered or bulleted lists. The unintended consequence was folks who were trying to adjust the positions of their notes would ocassionally attach a note to a dimension. The only way around this was to hold the shift key while moving a dimension, but you'd also lose the preview while dragging it.
SP3 adds a System option under Drawings. "Disable note merging when dragging." And its turned on by default, getting you back to pre-2010 behavior. If you want that functionality back simply uncheck it.
Remember, the squeaky wheel gets the grease. If there is something that could be better in SolidWorks send in your enhancement requests.
I had a support case today where a customer was unable to get his thread information or “hole callouts” from the hole wizard to show up in the dimension of his drawings. The hole was dimensioned correctly but the hole callout information was missing. Upon further investigation I discovered that the hole callout information is from a text file named “calloutformat.txt”. This file can be in any location as long as SolidWorks file location points to it. Mine was in the default file location.
Somehow the customers file became corrupt. The solution to the issue was for me to send him my hole callout text files. Once the customer replaced his hole callout files with my files his hole callouts worked without issue.
This got me interested in why this file exists and what it is used for. A little digging in SolidWorks help got me the answer. The file is there so we can set up hole callouts exactly as we want, or what our company standards dictate. If the default hole callout that SolidWorks gives you is not what you want edit it to fit your needs. To do this open the file in Notepad. You can now edit the definition for the Hole Callouts and create them exactly as you want. If you have created a custom set of Hole Wizard Standard you may also want to create a custom set of Hole Callouts to match it.
Using the code of the symbol library, you can position symbols and order them in the definition of each hole wizard type. For example, <MOD-DIAM> creates a diameter symbol. The end of the file contains text descriptions of the variables.
Don't forget that anytime you modify a standard SolidWorks file its important to back it up so if you reinstall and wipe out your directories it is maintained. If you have multiple users in your group this file should also be added to a shared location so everyone is working with the same one.
There is a great section in SolidWorks help that gives examples and definitions of all the options. Search for "Hole Callouts" and it should be the first article you find.
A question we get a lot on the support lines is “How do I dimension to the theoretical intersection of two lines?" If you use a sketch fillet it's really easy since SolidWorks automatically puts in a virtual sharp for you. But what if you didn’t use a sketch fillet? How come there isn’t a “Virtual Sharp” command within the sketching environment even though there is a whole section under Document Properties dedicated to controlling their appearance. The solution is simpler than the preceding introductory paragraph. Thanks to Stefanie for providing the screen captures and directions.
- Hold Ctrl and select the 2 lines as pictured below.
- Select the Point icon.
- A point/intersection will appear representing the virtual sharp.
Virtual sharps can be inserted into 2D sketches, 3D sketches and Drawing views. To change their appearance go to Tools/Options/Document Properties/ Virtual Sharps.