Category: Tip/Trick

SolidWorks quick tips and tricks.

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

Setting up and using SolidWorks Revision Tables faster

I am sometimes surprized by the limited the adoption of the SolidWorks Revision Table.  This is a powerful tool for drawings within SolidWorks.  The Revision Table allows the user to create a drawing template with an easily updateable revision block already included.  The user doesn’t have to use a potentially unstable Excel inserted OLE.  They also do not need a drawn revision block that requires significant labor in order to update and maintain.

The SolidWorks Revision Table is easy to insert in SolidWorks 2008.  With a drawing open, just go to Insert pulldown>Tables>Revision Table.  Within the Revision Table Pane, pick the appropriate revision template.  Choose any desired options for the table. Choose OK.  The Revision Table will automatically appear in upper right corner.  Save the drawing template for future use.  (See Help for instructions to place the Revision Table at other locations on the drawing.  Also, more steps are required in 2007 and prior; but, they are intuitive to follow and provide more on-screen control over the table’s location.)

Custom Revision Tables can be created to suit the companies specific needs.  Right click on the table to use the RMB menu to access functions that provide methods to modify the table.  When modifications are complete, use the RMB menu Save As option to save the new table as a table template for future use.

To add a revision, simply right click on the Revision Table.  Choose Revisions>Add Revision.  A new revision row will appear with the next revision inserted.  Simply double click any field to add or modify its value.  LMB click outside of the table to set the edits.

Of course, there is a simpler way to add revisions to the Revision Table!  I’ve created a macro that provides a form which allows the quick addition of revisions to the Revision Table.  It’s called RevBlockControl.  It is much faster than directly creating and entering all the rows and values.  It has been recently updated, so if you already use this macro, please consider using the latest version.

RevBlockControl Form

Sample image of the macro form

To use the macro, place it in the macros folder under the SolidWorks folder.  If it doesn’t exist, create it.  Within SolidWorks, assign a custom key stroke to the macro and/or create a toolbar icon location for it.

It can be used for a variety of revision table set-ups, including standard recommended ASME types.  It is limited to 5 columns, though it is customizable without editing the code or a complex .ini file.  If editing the code is desired, everything is spelled out with descriptions for easy of use.  In fact, the code can be quickly edited to allow the macro to drive the drawing’s “Revision” custom property.  Additionally, there is a small .ini included in this current version.  It is simply a list of initials used by the Rev By field.  Edit it with NOTEPAD to add and delete names that will automatically appear within the Rev By field.

Even without the RevBlockControl macro, the easy of use of the SolidWorks Revision Table is well worth the few minutes of effort to set it up on a template.  With the RevBlockControl macro, adding revisions to a Revision Table is so fast that it is almost effortless when compared to other type of revision blocks.

Control Root Size of Drafted Rib on Curved Surface

*This article makes some inaccurate statements regarding the capability of SolidWorks.  Please see the correction article for details.  Inaccurate statements have been crossed out.  The methodology described in this article should be referenced as an example of bad practice that should only be employed if traditional methods fail.  Edits to this article appear in this color.*
*Additional comment: this article does demonstration a good method for getting a line along a curved surface into a sketch. *

Good mold design means that one must take care to control the root width of a rib.  How does one do this if the rib is based on a curved (non-prismatic) surface? 

SolidWorks has many powerful features for making injection molding parts.  It has both rib and draft features.  Unfortunately, these two features together have one important limitation.  When applying a draft to a rib based on a curved surface, SolidWorks does not allow the user to hold the root width of that rib.  SolidWorks requires a prismatic surface to use as a neutral plane from which to start a draft.  This means in this case, the draft can only be started from the top of the rib, not its root.  If one wishes to hold the rib root constant along a curved surface, one cannot use the rib or the draft features.

SolidWorks does have an arsenal of other features and tools to allow one to build an alternative strategy to workaround this limitation.  

Basic shelled part with curved surface

This first figure shows a fairly simply shelled injection molded part with a complex curved surface.  To make drafted ribs using this method, first create an axis that can be used as an directional guide. You can choose to use features on the part itself for this purpose, instead. I prefer to create a special sketch at the location where I plan to add a boss.  Regardless of the method used, the directional guide should be parallel to the direction planned for the ribs.

 Setup Sketch for Directional Guide

The second step is to start a new sketch above the curved surface.  In that sketch, draw the outline of the rib.

Sketch outline of ribs

If there is a series of ribs needed in one direction, try creating a sketch pattern the other instances.  Make sure to turn sketch entities of the other instances into construction lines.

Project outline using Split Line

Use Split Line to project that outline onto the curved surface.  Split Line will only project one contour per sketch.  This is why it is important to turn all other instances of the rib into construction lines.  Having those other instances pre-drawn will save time when making the other ribs (covered in Part 2 of this article). 

Next, start a 3DSketch.  Use Convert Entitles to bring the Split Line curves into the sketch.  Drag the end points of the curves so they are coincident (on the surface) of the outside surface of the outer walls, or some othe appropriate location.  Then, close the contour by drawing lines to connect the curves at each end. 

Convert split line edges in 3DSketch

Extrude this sketch.  Use the previously drawn axis from the first sketch as the direction.  Use the top surface of the cavity (or whatever is appropriate) as up-to-surface entity.  Turn on Draft and specify the desired angle.  Here’s the funny part.  Be sure to extrude a small amount (smaller than the wall thickness of the part) in the other direction without draft.   If this isn’t done, a zero-point error will pop up preventing the completion of this step.

Use previous setup to set extrude of 3DSketch

The end result will be a drafted rib with a controlled root width.

Final result

Part 2 of this article will detail how to create repeated and crossing ribs using this same technique.  Again, please note this is not a best practice method.  See the correction article for details.

Dual Dimensioning and ASME Y14.5M-1994

This entry is part 2 of 8 in the series Dimensions and Tolerances

Dual dimensioning is the drafting practice of using multiple units of measure in a dimension in the same direction of a feature.  SolidWorks and many other CAD programs support dual dimensioning.  This support is usually a little quirky.  It’s actually not  the fault of the CAD application.  At one point, it was a surprize to me (and often is to others too) that no current drafting standard actually supports dual dimensioning.  In retrospect, this makes perfect sense.

My experience is with ASME Y14.5M-1994.  When invoking ASME Y14.5M-1994 (or even ANSI Y14.5M-1982), one will find that rules regarding dual dimensions do not exist.  ANSI Y14.5M-1982 does mention in its appendix that support for dual dimension no longer exists in the standard.  This is apparently because it was mentioned in a previous version.  That said, dual dimensioning has never really ever been allowed by any incarnation of Y14.5.  This is because of very specific wording under the standard’s Fundamental Rules.  The wording may vary between versions, but carries the same meaning in all versions.  In ASME Y14.5M, that wording is as such in 1.4(d), “Dimensions shall be selected and arranged to suit the function and mating relationship of a part and shall not be subject to more than one interpretation.”  (Support for dual dimensions in pre-1982 versions was a mistake that was likely political in nature.)

General practice in the use of dual dimensions is that they are of equal importance to the primary dimension.  This creates issues in that it allows for more than one interpretation of the dimension.  It is nearly impossible for nominals and tolerance ranges to be identical between units of measure.  This means that the dual dimension tolerance range is usually resized to fit within the tolerance range of the primary unit of measure.  This creates a situation where the dimension has more than one interpretation, which is specifically prohibited by 1.4(d).  The conclusion that can be drawn from this is that dual dimensions are actually not allowed by ASME Y14.5M-1994.  This is the hard argument against the use of dual dimensions.  I could end this article right here.  However, I will also explore the soft arguments against their use.

ASME Y14.100-2004 paragraph 4.32.3 uses soft language to discourage the practice of converting inch to metric and vise verse (“should not be used”).  This is known as soft conversion.  This is not an outright prohibition against dual dimensioning by itself. However, the practice of soft conversion is integral to using dual dimensions.  With this practice discouraged, dual dimensioning is also discouraged.

ASME Y14.5M-1994 defines a reference dimension as such,

“A dimension usually without tolerance, used for information purposes only. A reference dim is a repeat of a dimension or is derived from other values shown on the drawing or on related drawings. It is considered auxiliary information and does not govern production or inspection operations.”

By definition of reference dimensions, dual dimensions must be treated as reference dimensions. However, anyone who uses them knows this is generally not their intent. As generally intended, dual dimensions are disallowed unless they are considered reference only.

The final soft argument is gleamed in the wording of ASME Y14.5M-1994 paragraph 1.5.  This paragraph assumes dual dimensions are not in use.  For example it begins one paragraph as so, “Where some inch dimensions are shown on a millimeter-dimensioned drawing…”.  It never then says “Where many inch dims are used on a metric drawing….” This is not a specific exclusion, but should be noted for its wording. It does allow for the use of both inch and metric units on the same drawing, but not multiple values of dimensions for the same features.

With all of these arguments aside, CAD applications do attempt to accommodate users who feel they need this capability.  However, if used, caution must be exercised.  Handling of dual dimensions by CAD (and common practice) can create confusion on a drawing, particularly if the software assumes values for the dual dimensions and its tolerances.

In the effort to avoid issues and violations of the standards, it is my opinion that if dual dimensions are used, they should be noted as for reference only on the drawing.  This can be accomplished by adding a note similar to “DUAL DIMENSIONS IN BRACKETS ARE FOR REFERENCE ONLY.”  This avoids problems caused by multiple interpretations for dimensions.  Of course, over use of reference dimensions is also discouraged by ASME Y14.5M-1994. But hey, who’s it hurting?

For SolidWorks, dual dimensions on a drawing may be employed by going to Tools>Options>Document Properties>Detailing and checking Dual dimensions display.  Also at that location is the choice to display the dual dimension on top, bottom, left or right of the primary dimension.  These are SolidWorks 2007 instructions (other versions of SolidWorks should be similar).

I did make a sample SolidWorks macro that will turn on dual dimensions for a drawing and automatically set them to display on the bottom (default is top).  This example macro can be downloaded here.  It can be modified to use any settings as default.

For the record, this article was inspired by multiple posts on various SolidWorks related forums over the past few months such as these at SW Forums, eng-tips.com, and Pro/E discussion at eng-tips.com.

Workaround to edit Macros that are locked on network drive

Question:  I have macros on a network drive and need to edit them.  Unfortunately, someone has them locked (open).  How do I unlock them without going to that computer to manually unload the macros?

Answer: There is a live workaround.  While you cannot edit the files while locked, you can change their folder name! This allows for a sneaky little trick that doesn’t require going to the offending computer.

Simply rename the folder on the network drive where the macros are located. Then copy that folder (files and all) to the same drive. Rename the new folder to be the same name as before the original folder was renamed.

The macros in the old folder with the changed name will still be locked out, but the macros in the new folder with the original name will be free to edit!

In a day or so, the files in the old folder will be unlocked again.  Simply delete the old folder at that time.

Addendum: It should be noted that this method will not always work.  However, it is worth a try before taking any other action.

Better Modeling using Pencil and Paper

I am finding more and more posts on engineering related forums as well as discussions with industry professionals that cannot believe that designers and engineers have little to no idea how to sketch using a pencil and paper.

Personally, sketching helps me reduce my modeling time anywhere from 20-50% while at the same time increasing the simplicity and accuracy of my model.  In my Advanced Modeling course at NTI I start off the course by asking the students to define advanced modeling.  Those who do not know me yet will answer with functions like Surfacing, Sweeps, Lofts, Sheet Metal, Weldment so on and so forth.

Then I pull out my soap box and tell the students that these are actually industry specific standard tools.  If you are working on sheet metal day in and day out then those are generally the core set of tools you use son on and so forth.  Same goes for Mold Tools.

The next part of my presentation talks about advanced modeling being about modeling using the most basic tools possible to accomplish a manufacturable component, assembly that 2 years down the road the next newbie can immediately open and make the necessary changes for the next design.  I talk about taking the time to model as best you can in a manner that will allow you to import you model dimensions to the drawing to save time in the detailing process.  Model so that your drafts, fillets, chamfers (dare I say it “extruded text”) are at the bottom of the feature manager tree so they can be easily suppressed.  Use the hole wizard to aid not only in assembly but also use you companies standard hole callout format.  Try to limit the parent child nightmare by relating back to datum planes, origin or you base feature.  These are tangible items in which i can immediately show the results and demonstrate the value.

Being able to sketch your part before modeling is proving to be more of a challenge.  I cannot tell you how much time I have saved throughout my career by sketching before I model.  It is a great way to spend those countless hours in drawn out design reviews (cat fights).

What value do I find in Sketching?  It allows me to envision how my model will be constructed (is this a cast to machined part? will this become a progressive die stamped part? how can I ensure my design intend in understandable?), add notes to features that may associate to other parts of the assembly (this hole is related to part B, the connection is a shaft the will be pressed into 2 bearing what was that fit again?  Oh yeah it is right here in my sketch), list our drafts, minimum radii, wall thickness, materials to select from, I can add all kinds of research to a sketch that will reduce my time at the computer and increase my productivity while I am at it.

This is proving to be a challenge to convey to students.  They want to work on the computer all the time.  I even talk about my time in Florida (the highest number of lightning strikes per inch capital of the world) and how there is often times you can not have a computer with you.  Or how about when one of your machines is on the brink of failure but we can only take it offline for a given amount of time to reverse engineering the no longer existing replacement parts needed to over haul the machine.

Anyone else in the Legion have some examples of how they use sketching to improve modeling productivity?  Any one out there think that sketching is the dumbest thing next to the pet rock.  Let me know.  My student will benefit from all views.