Category: How-To

SolidWorks how-to guides

SolidWorks 2009 Title Block management

SolidWorks 2009 makes further inroads into the area of drawing control.  In the past, they added sheet formats, revision tables, BOM improvements, and links to model properties.  The move to improve drawing control has been slow, often in baby steps.  The newest control addition is another such baby step.  SolidWorks now allows users to specify title block fields for direct entry.  This mean, you just double click on the particular title block fields and fill-in their content quickly without any other functions.  This functionality is nice, but given the extensive use of model and/or drawing custom properties to automatically fill in title block fields, I’m not sure how truly useful this new Title Block management really is for most users (at least in its current state).  I can imagine this might benefit users who rely heavily on model custom properties, as they may find it useful to not rely on a custom property for the drawing’s Drawn/Date By fields (where the drafter is a different person than the solid model designer). 

Using the Title Block Manager

The new functionality is easy to use, and not difficult to set up for an existing title block.

  1. To set up, open a drawing sheet or template.
  2. RMB click the sheet format in the FeatureManager.
  3. Select Define Title Block. This will re-center the view window on the drawing’s lower right (presumably the title block location).  A grab-able black rectangle box appears at this corner of the drawing.Select fields
  4. Resize the box to fit roughly around the title block area.
  5. LMB click on any single-line annotation note that is meant to be filled in manually for each drawing.  Each field will highlight blue, and be added to a list in the FeatuerManager pane.
  6. Select OK.Using the field
  7. Once satisfied with the set up, save as a drawing template.

Then, when in a new drawing, just LMB double-click to activate the field and enter the desired data.   As shown here, setting up and using this new functionality to control drawing title blocks is very easy.  It may be most useful for those setting up new title blocks; perhaps this is best for those companies upgrading from 2D CAD applications.

Drawing Revisions and PDMWorks (Part 2: Automatic Revisions)

With PDMWorks, it is possible to automatically revise a drawing’s title block and revision block upon check in.  Three things are necessary to use this functionality.  First, the drawing template will need to employ a SolidWorks Revision Table.  If someone is not familiar with how to set up revision tables, please see my previous article: Settings Up and Using SolidWorks Revision Tables faster. Second, the drawing template’s title block will need an annotation note that is linked to the custom property “Revision”.  If someone is not familiar with how to link annotation notes to custom properties, please see my previous articles about this subject:Introduction to SolidWorks Custom Properties.  Third activate the revision automation feature within the PDMWork’s VaultAdmin tool.  Of course, this will require Vault Administrator access to the VaultAdmin. The setting is found under the Revision Table tab in the General section, called “Enable Revision Table”.

Once these three items are set up, drawings will automatically revise upon check in, with updated revision and title blocks.  Control over what appears in the added revision row is within the check-in screen itself when the drawing is checked in.  Further controls can be set up to limit or automate the value for revisions so that no mistakes can be made regarding the revision level of the check-in.  Within the VaultAdmin, there is even the ability to control the number of revisions visible on a drawing.  Utilizing this set up can save substantial time and eliminate potential check-in revision identification errors.

Drawing Template with Two Different Sheet Formats (Part 2)

UPDATE for SolidWorks 2014: The following protocol is no longer necessary to achieve a different sheet format for addition sheets on a drawing.  Please see 2014 What’s New in SolidWorks – Sheet Formats for current information.

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Here is the [no-longer-necessary] protocol to set up a Drawing Template so that it can use two completely different Sheet Formats without requiring any additional action by the user when they start a new drawing.

This protocol tricks SolidWorks into having a Drawing Template use one Sheet Format for sheet 1, but also to have a different Sheet Format as the default for any added sheets.  It does this by swapping around the names of the Sheet Format files.

This allows a CAD Administrator to set up their Drawing Templates to be ASME compliant by automatically calling up the simplified title block when additional sheets are added to a drawing.

Instructions

In Windows Explorer:

1. Save a backup copy of the current sheet 1 and multi-sheet Sheet Format files.  Also, save a backup copy of your Drawing Template.

2. Rename multi-sheet file, such as adding an underscore in front of its name.  For example, if your multi-sheet file is named “C-SIZE-SECOND.slddrt”, rename it to “_C-SIZE-SECOND.slddrt”.

3. Rename sheet 1 file so that is has the original name of the multi-sheet file.  For example, if your sheet 1 file is “C-SIZE.slddrt”, rename it to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

4. Start SolidWorks.

5. Open your Drawing Template.

6. Load your renamed sheet 1 Sheet Format.  In the example above, this would be “C-SIZE-SECOND.slddrt”.  The result should be a drawing that shows your sheet 1.

7. Save your Drawing Template.

8. Close SolidWorks

In Windows Explorer:

9. Rename sheet 1 to its original name.  In the example above, rename the “C-SIZE-SECOND.slddrt” file back to “C-SIZE.slddrt”.

10. Rename your original multi-sheet file to its original name.  In the example above, rename “_C-SIZE-SECOND.slddrt” to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

11. Start SolidWorks.

12. Test results by starting a new drawing using the same Drawing Template.  Sheet 1 should appear on sheet 1.

13. Create sheet 2.  The multi-sheet format should appear on sheet 2.

For best results, uncheck “Show sheet format dialog on add new sheet” in Tools pulldown>Options…>System Options tab>Drawings.

The limitation of this method is when the administrator wishes to change sheet 1 of the Drawing Template, they will have to replicate these steps each time.  That doesn’t happen often and well worth the savings in time produced by implementing this method within the Drawing Template.

Additional keywords: 2 title blocks drawing

Drawing Template with Two Different Sheet Formats (Part 1)

A long sought after function in SolidWorks that has gone pretty much ignored is allowing users to set up Drawing Templates with two different Sheet Formats (one for Sheet 1 of X and one for all other X of X sheets).   [In the past, m]ost of us just had to  directly pick and load the separate X of X sheet when we add a sheet to a drawing.

Some half solutions do did exist to get around the limitation.  I have seen one hack that involves using the X of X sheet Sheet Format as the default sheet format with sheet 1 of the Template itself simply having addition entities around the Sheet Format entities to form the complete sheet 1 of X “format”.   Another way is was to have two sheets already present in the Drawing Template, each one with its own Sheet Format; then delete sheet 2 when it is not used.  No more half steps!

There is a way to have two completely different Sheet Formats embedded into a Drawing Template without having additional sheets already present.  I am currently working on writing up the protocol. I will post the steps on Thursday 7/17/08 (Instructions are now available here).  The protocol is not complex as far as I can tell.  I just wish to thoroughly experiment and test it before posting.  Stay tuned.  And, if you know of other ways do to this, then please post your methods (or links to them) here so everyone can compare notes.  Who knows, maybe someone else has already published something about this  I just know I’ve not seen anything in any other online resources, which is why I’m fairly excited about making this method available.

UPDATE for SolidWorks 2014

SolidWorks 2014 now has a second sheet setting in Document Properties. Fancy workarounds are no longer necessary.  Please see  2014 What’s New in SolidWorks – Sheet Formats.

Drawing and Viewport Backgrounds

SolidWorks 2008 introduced the ability to control the drawing background.  This was made obvious with the notorious implementation of the Crinkled Paper image that now dons SW 2008 on-screen display of drawings.  This image is kinda cool, but also not really all that professional.  It is an unusual and quirky choice for a default image, to say the least.  Just as quirky is that fact the user cannot choose to print their drawing with that background included.  This makes the whole thing seem rather silly.  Regardless, there is a fairly easy method to change this image.  Instructions to change this image appear latter in this article.  Also included are the instructions to simply turn this function off.  Also included at the end of this article are locations where some background images are available for download.

Before SW 2008, the user only had the ability to set a solid color as the drawing background.  The user did have capabilities to control the viewport background, which also appears underneath the drawing background.  The abillity to control this viewport background has improved over the years.  In the early days, one could only set the color.  Then SW wowwed us with transitional coloration.  Later, the user could display an image as the background.  Instructions on how to apply an image to the viewport backaround appear later in this article.

Instructions to change the drawing background in SW 2008

1. Obtain or create a new Bitmap (.bmp) image for use as the background. For best results, the .bmp should be a pixel size that is similar to the current SW 2008 backgruond image (sheetbackground1.bmp).  Also, be sure the background image is light or ghost-like so that it does not obscure the drawing itself.
2.  Shutdown SolidWorks, if not already.
3. Goto the SolidWorks\data\Images\drawings folder in Windows Explorer. Note: this folder location may vary some between systems at the “Solidworks” level.
4. Rename the standard sheetbackground1.bmp to back it up.
5. Copy the new sheetbackground1.bmp into that folder.
6. Start SolidWorks and open a drawing to confirm.

Instructions to turn off the drawing background image in SW 2008

1. Start SolidWorks.
2. Goto pulldown Tools/Options…/System Options tab.
3. Select Colors in the left selection list.
4. Check the box of “Use specified color for drawings paper color”.
5. If you wish to change the default paper color, select “Drawings, Paper Color” in the “Color scheme settings” list and LMB click on the “Edit…” button to the right. This brings up a window where you can select another color. Pick “OK” button of that window to return to System Options.
6. Pick “OK” button of the System Options to implement the changes.
7. Open a drawing to confirm changes.

Instructions use an image as the viewport background for SW 2006 and above

1. Identify which image you’d like to use as a viewport background.  Note: drawing background images from SW 2008 can also be used as viewport backgrounds in SW 2006/7.
2. Start SolidWorks.
3. Goto pulldown Tools/Options…/System Options tab.
4. Select Colors in the left selection list.
5. Select the option to use an Image file under “Background appearance”. The exact name and placement of this selection may vary between versions of SolidWorks. Look for the field that allows the entry of a file name and its associated browse button (three dots).
6. Browse to the location of the image to be used as the background, and select the image file. Pick “OK” or “Open”.
7. Pick “OK” to accept the change in System Options.
8. Open a drawing to confirm change.

Locations to find drawing backgrounds

Hole Callouts: Why is THRU sometimes THRU ALL?

This entry is part 3 of 4 in the series Hole Callouts

Question: On a drawing, when adding a callout to a simple through hole or thread, SOLIDWORKS will sometimes add “THRU” and other times add “THRU ALL”.  Why does SolidWorks sometimes add “THRU ALL” in such cases, even though the hole is obviously just “THRU”  (“THRU ALL” being through multiple features and “THRU” being through just one feature.)

Two words: Design Intent.  SOLIDWORKS has powerful modelling tools that allow the user to establish design intent.  In the case of through holes and threads, this design intent is created by the user’s choice on how to make that hole through (its End Condition).

Notice, if a hole is added to a model where the end condition is blind, but the depth of that blind hole cuts through the part, the hole callout on the drawing will show stated depth and not the fact that the hole is through.  Here, the design intent is that the hole shall be cut to a particular depth regardless of the fact that the hole ends up being through the part.

By instinct, many of us pick “Through All” as our end condition for a hole.  However, SOLIDWORKS interprets this as the user’s design intent to make the hole through every feature, so the drawing’s hole callout is “THRU ALL” even though there is only one feature being drilled through.  To capture design intent of “THRU”, the end condition of the hole must be “Up to Next”. This tells SOLIDWORKS the design intent is that hole is only through the immediate feature regardless of how many features it may intercept.

For threads, both end conditions may be set to “Up to Next” for the design intent to be fully captured so that both bore and thread are called-out as “THRU” on the drawing.  A side note, thread callouts may still show depth, even if “Up to Next” is selected.  Be mindful of this.

If drawings already exist with non-modified hole callouts, simply updating the model will usually update the drawing callouts.