Category: How-To

SolidWorks how-to guides

Foreshortened Diameter Styles

SolidWorks supports two styles for foreshortened linear diameter dimensions.  The default style is the traditional zigzagged dimension line on the foreshortened leg.  The other style is the often preferred double arrow.  Only one style may be used on any particular drawing.  This is because the style is set in Document Properties.

Foreshotening styles

Instructions for SolidWorks 2008 and prior:

  1. Open a drawing.
  2. Goto Tools pulldown>Options>Document Properties tab>Arrows heading.
  3. The last section of the Arrows window is called Foreshortened diameter.  Here, simply select the style, and then OK to exit.

Instructions for SolidWorks 2009 or later:

  1. Opening a drawing
  2. Goto Tools pulldown>Options>Document Properties tab
  3. Click on the Dimensions heading and the Diameter subheading.
  4. The last section of the Arrows window is called Foreshortened.  Here, simply select the style, and then OK to exit.

The change will immediately become effective for all foreshorten linear diameter dimensions on the drawing.

Color for non inserted dimensions

SolidWorks has many default colors for different types of dimensions.  On drawings, the two main types of dimensions are inserted (driving) and non inserted (driven).  Inserted dimensions are called such because they are inserted from the model.  Non inserted dimensions are created within the drawing itself.  I’m not going to get into the philosophies about which is better to use and when.  Let’s just stick to the topic that many times both are necessary on a drawing, and that they appear as two difference colors. Inserted dimensions are black and non inserted dimensions are grey, by default.

A problem pops up when using or printing the drawing while in Color Display Mode is on.  When this mode is turned off, all dimensions appear black, but so does everything else, including watermarks or lines on special layers.  So, many of us rely on the Color Display Mode.  When this mode is turned on, the user gets their colors right for other lines, but dimensions appear as both black and grey.  This can send a confusing message to someone who must later read the drawing.   Also, on some printers, the grey color may be washed out and unreadable.

Example of different colors

So, I have a quick trick to overcome this issue.  Simply change the color for non inserted dimensions within the System Options.   What color to use?  Well, if one still wants to know the difference between inserted and non inserted dimensions when editing the drawing, I recommend not picking black.  Instead pick the darkest grey available.  This will allow you to see the difference in SolidWorks, but such a difference will not be obvious in any printouts or PDFs.

To make this change in SolidWorks, goto Tools pulldown>System Options>Color heading.   In the Color schemes settings box, select Dimensions, Non Imported (driven).  Click the Edit button.  A traditional Windows color palette window will appear.  Use this window to create a very dark grey color and then assign it to one of the slots in the Custom colors area.  Choose that color as the setting and click OK to exit.  Then click OK in System Options to implement the change.

Color change location

All inserted dimensions will continue to be black, and non inserted dimensions will now be that dark grey.   Since this is System Options setting, it affects any drawing that is opened without having to enter the Document Properties area every time.  I’ve personally used this trick successfully for a long time.

Radius and Diameter Dimensions (switching these in SW 2009)

It doesn’t matter if the dimension starts off as a radius, diameter, or a linear diameter dimension (on a drawing in a model).  One can become another quickly in SolidWorks 2009.

Step 1:  To change a radius to a diameter, RMB click on the radius dimension.  Choose Display Options>Display as a Diameter.

Step 2:  To change a diameter dimension into a linear diameter dimension, RMB click on the diameter dimension.  Choose Display Options>Display as linear.

Unfortunately, there is no way to shortcut these steps from a radius dimension to a linear diameter dimension.  If starting out as a radius, both of these steps will need to be followed in succession to get a linear diameter dimension.  Same goes for the reverse.

One word of caution when switching to a linear diameter dimension though; it will often not come in aligned to the Y or X axis, which may render it unuseful for certain circumstances.

Foreshortened Diameter Dimension

Foreshortened linear diameter dimensions are not specifically supported by ASME Y14.5M-1994.  I don’t know if “ASME Y14.5M-2009” will have such support added.  Even if not, there is a common practice of showing foreshortened diameters.  SolidWorks supports the two most common delineations for these.

To have a foreshortened diameter dimension, the diameter being dimensioned will have to be cut off in the view.  This means effective use of these is pretty much limited to detail views, since this is likely to be the only place one would normally use such dimensions.  I may try to experiment in the future to see just how far I can stretch SolidWorks functionality in this area, but for this article, I’m going to stick to the basics.  Please note that these instructions are SolidWorks 2009 based.  Steps will be similar in older versions, but may not be exactly the same.  They will be close enough to make this a good guide, though.

Preparation

To employ a foreshortened diameter dimension, there is some preparation needed within the model.  You cannot just insert your model into a drawing and add a non imported dimension onto a circular feature.  Because of the way Hole Wizard functions, foreshortening will also not work for holes created with it. Why?  I’m not sure as to the reasoning.  I just know SolidWorks only enables this function for imported dimensions (dimensions inserted from model).

  1. Start a sketch in your model.  This sketch will become your feature.
  2. Draw a circle.
  3. Dimension that circle as a linear diameter dimension.  This will not work if the dimension is radial.
  4. Make sure this dimension is set as mark for drawing.
  5. Create a feature from the sketch.

On the drawing

Insert the model onto a drawing.  Create a detail view which cuts across a circular feature.

Cutting the Detail View

Detail A

Once the drawing is set up, here are the steps.

  1. If the center of the circle appears in the detail, select the detail view by LMB clicking it.  If the center does not appear in the detail, then select the parent view instead.
  2. Insert model items.  This can be done by Insert pulldown>Model Items.  One of the dimensions to appear will be the diameter of the circular feature.
  3. Click OK in the PropertiesManager Pane to accept and close Model Items panel.  If already in the detail view, you are done.  The dimension will appear as a foreshortened linear diameter dimension.  However, if working in the parent view, a few more steps are required to get the desired effect.
  4. Hold down the SHIFT key.  Select the diameter dimension by clicking and hold the LMB over it.
  5. Drag the dimension in the detail view.  Let go of the LMB and SHIFT key.  This will copy your dimension into the detail view. The dimension will appear as a foreshortened linear diameter dimension.
  6. Delete the dimension from the parent view.

What’s next?

SolidWorks is very particular about how it allows foreshortened linear diameter dimensions.  These steps must be followed exactly in the manner described here.  I wish SolidWorks made it easy to implement foreshortened diameter dimensions, including allowing them for non inserted dimensions.

Future articles on this topic will discuss styles of foreshortened delineation (how to get double arrows instead of the zigzag dimension line).  It will also discuss one work around so foreshortening can be applied to other types of linear dimensions, producing a result sometimes called clipped dimensions.

Foreshortened Radius

Foreshortening a radius dimension on a drawing is easy.  The option to foreshorten a radius is found when the radius dimension is highlighted by looking under the heading of Display Options in the PropertiesManager pane.  (Note: this foreshortening option will not be available if dimensioning a full diameter within the view current view, even if the dimension is shown as a radius.)    Once this option is chosen, the radius dimension will appear foreshortened with a zigzag radial line.  The user can then adjust the shape and location of the zigzags, as desired.

 

Options

 

This is easy enough.  I am covering this basic how-to tip as a lead-in for the more complicated task of foreshortening diameter dimension in an upcoming article.

Measure that Mate (Why are results different?)

I was recently asked,

“I did a check where the distance mate value and the measurement for the same features shows two markedly different values.  Have you ever seen anything like this?”

Distance Mate Result

This individual wondered how it was possible that his measurement of two associated features was different than the dimension he entered for the distance mate assigned to those two features.

Measurement Results

My reply was pragmatic.

“Without seeing the model directly, it’s hard to confirm the error.  However, I have found that whenever SolidWorks gives me a number and it doesn’t make sense, it is due to something the user is doing or some misinterpretation of the data.  This causes me to try to investigate when such issues arise by first considering what the user is doing.

“In this case, I’m assuming you are measuring from the center of the circle to the flat face.  However, I notice that your mate is set up face to face. I’m guessing SolidWorks is mating your hole based on the closest point of the circular face, and not the hole’s center.

“To fix this, use the temporary axis of the hole as the selected entity for your mate instead of the hole’s face.”

This individual followed my advice and was able to eliminate the apparent discrepancy.  In general, it is a good idea to check look at how SolidWorks (or any software) functions in order to understand why something is happening.