Category: Drawing

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 Revisions and PDMWorks (Part 1: Letter Revision Identifiers)

Whether using actual drawings or relying on the model, and whether using a highly controlled documentation system or nearly completely uncontrolled, one will find revisions are necessary.   It is important to use them consistently.  It is important to make sure each time another person sees a drawing or model, they understand which revision is in front of them.  It is important not to reuse revisions. If there is a working copy that is incomplete, preliminary or draft, then stating such directly on the document is very important.

Also important is avoiding interpretation confusion.  If using letters to represent revision iterations, avoid using letters that resemble numbers or that can have alternative meanings.  ASME Y14.35M-1997 states that I, O, Q, S, X and Z should not be used as revision letters.  In fact, other ASME engineering drawing standards also forbid the use of these letters for other purposes as well.  The reason is that I, O, Q, S, and Z all can be misinterpreted as numbers 1, 0, 5 and 2.  When X is used, it looks like a field that requires further input.

These rules where written before the Information Age (wiki) and our reliance on computer databases, back when documentation relied on handwriting.  However, these rules are just as important in our current age as they have ever been before.  Many different types of computer fonts exist.  What looks like a 1 in one font will look like an I in another.  Even with my 20/20 vision, I will confuse S’s with 5’s in small sizes in certain common fonts.  Also, transcription errors still enter the picture, as a human who does not have direct access to the electronic database is usually involved at some point.

PDMWorks (soon to be renamed to SolidWorks Workgroup PDM by SolidWorks Corp) automatically assigns revisions to documents when they are checked-in.  There are options for the PDMWorks Administrator to use dumb ranges, or to establish a list of revision identifiers from which to pull.  Unfortunately, when using letters, PDMWorks does not automatically disregard the taboo letters.  So, I’ve made an Excel file with a list of allowed revision letters.  It can be copy-and-pasted directly into PDMWorks VaultAdmin’s Revision Scheme Listing fields.  It is available here: Allowed Revision List.

Part 2 of this article series will address using PDMWorks ability to automatically revise drawings upon check-in.

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.

SolidWorks 2009 is slated to introduce Slots functionality

At SolidWorks World 2008 (SWW8) we saw confirmation of a rumor.  SolidWorks 2009 would have the capability to add slot holes to parts.  This is a long sought after function that some would say has been missing along.  As demonstrated, the slot hole was not a special feature.  It was a sketch tool! Some may not initially like this, preferring slot holes to be their own discrete type of feature.  Others may prefer creating slots with a special sketch tool.

The SWW8 demonstration showed the presenter starting a sketch, picking the slot tool.  This allowed him to draw just a construction line with two LMB clicks.  The slot form automatically formed as though it was a capped offset from the initial construction line.  One more click set the sketch entities for the slot.  It appeared to be easy and painless.  I presume dimensioning of the slot within the sketch would be similar to current methods for similar sets of entities in the current version of SolidWorks.

The advantage to the slot function as a sketch tool is that user can actually create either an extrude or cut-extrude with the same tool.  So, not only are slot holes supported, but so is their opposite and positive counterpart.  As long as SolidWorks allows the user to dimension the slot hole on the drawing with the Hold Callout function, I do not have any major issues with this.  A mild criticism is that this method is a kin to how holes were made in the earliest SolidWorks versions, long before Hole Wizard, and presumably even before those “legacy holes”.  Perhaps this is just the first volley in a long series of improvements as we work our way to a Slot Wizard?  Maybe not.

However, some users might be expecting slot holes to be a feature of their own.  I cannot fully imagine how SolidWorks might accomplish this.  Maybe special one-off sketches are required, with sizes regulated with a Property Manager, similar to Hole Wizard holes.  Thinking of this, I can imagine that it would be nice to have some feature level control over slots so that they can be automatically sized when associated with a particular fastener within an assembly.

As far as dimensioning for slot holes on drawings, I did participate in early questionnaires regarding how this should be done.  I dutifully pulled my advice from ASME Y14.5M-1994, with special attention to Fig 1-35(b).  I also stated that I preferred centermarks to be at the center of slot by default (again referencing Fig 1-35(b)).  This will allow the quickest and simplest scheme to specify a slot hole.  This brings to mind a question.  If Hole Callout does callout slot holes this way, what will it do for extruded shapes that use a slot sketch?  There is no standard for this in ASME as far as I can tell, other than just directly dimensioning the feature.

There is one major point of concern.  How does this function translate into model assemblies?  Does SolidWorks 2009 quickly identify the slot hole center when smartmating a fastener at that location?  Right now, I always groan when I have to mate a screw to a slot because so much has to be done directly by me.  Update: something as simple as a temporary axis at the center of slot hole will be enough to address this issue, I believe.

One minor question of mine is how would slot sketch entities be handled within a sketch?  I think it would be best if they are recognized collectively as a slot, but can also be “exploded” into individual entities when other shapes based on the initial slot are desired.

I am looking forward to regularly using the new Slot functionality.  It promises to be a great timesaver that is well overdue.

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