Category: Drawing

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.

Foreshortening Dimensions (Radial, not linear)

[Updated to address changes in SOLIDWORKS 2016]

SOLIDWORKS provides for the foreshortening of diameters and radii dimensions.  Older releases of SOLIDWORKS didn’t allow for the foreshortening of linear dimensions (or clipped dimensions), except in break views where both ends of the dimension are visible.  When I first encountered this limitation years ago, I was concerned that SOLIDWORKS developers just simply overlooked this functionality.  After all, if one can foreshorten a radius, then why not a linear dimension?  I was even sure I could find examples of this already being done on other drawings in detail views.  I was trying to use an open ended dimension line with double arrows on the open end.  I may have actually used this method a couple of times back in my AutoCAD days.

But what didn’t SOLIDWORKS support this for many years?  The lack of foreshortened linear dimensions can be understood by reading ASME Y14.5M-1994 paragraph 1.8.2.2.  This paragraph established the foreshortening of radii.  Its title Foreshortened Radii seems to preclude these methods for linear dimensions.  But why?

The clue is the intent.  1.8.2.2. states that if the center of a radius is outside the drawing or interferes with another view, the radius dimension may be foreshortened.  Strangely enough, paragraph 1.8.2.2 does not specifically describe the just how foreshortening is demonstrated, other than to say the dimension line is radial to the arc.  It does reference a figure that shows radii centers repositioned with zigzagged radial and coordinate dimension lines.  The key is that the center of the radius is still within view.  The dimensions have known termination at both ends.

Allowed foreshortening of radial dimensions

There is an issue with using this methodology on any dimensions where the termination of both ends is not clearly shown.  Without both ends of the dimension in view (or known through some other way), there is no established way to determine where the dimension’s open end terminates.  It is an incomplete specification.  In other words, if I have a detail view and attempt to dimension to a feature not in that detail, the fabricator does not know the location of the other end of that dimension.  SOLIDWORKS previous limitation was not really a limitation after all.  It follows the drafting standards in a very logical way.

Disallowed foreshortening and diameter forshortening

Another thing SOLIDWORKS allows is the foreshortening of diameters.  Although this is not directly supported by the standards, it is common practice.  Unlike the foreshortening of linear dimensions, foreshortened diameters make sense since the other end of the dimension is known, even if it is not shown.  I’ll address foreshortened diameters in more detail a future article.

As of SOLIDWORKS 2016, foreshorten of linear dimensions is supported without restriction.  This was added for customers who still need methods to clip dimensions regardless to the issues mentioned above.

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.

SolidWorks Drawings ER Blitz – SW Drawing Forum

There’s something going on over at the SolidWorks Drawings Discussion Forum.  There has been an on-going project consisting of users working together to form a list of requests to improve SolidWorks’ drawing functionality.  It all started out with a posted message that was simple, yet poignant by user RYAN W.

When is solidworks ever going to focus on drawings for a new release? Of all the parts in SW I think it needs the most improvement. When ever I find a bug or have a problem in SW it usually is in drawings. I think it would be great to have a new release focus on this area.

From there, the discussion evolved.  Users started going into what they would like to see added to SolidWorks’ drawing functionality.  Others brought up bugs they found.  Somewhere in the discussion, Dwight Livingston took the baton.  He compiled list of eighteen improvements from everyone’s comments.  It included requests such “Create option to attach the ASME symbol for ALL AROUND to the bend of a leader”, “Change SW tables to have basic spreadsheet functions, without MS Excel”, “Create option to add a new centermark to an existing centermark group”, and “Create feature to embed custom symbols in drawing files”, just to name a few. 

This list has received considerable enthusiasm and has taken on a life of its own; it grew in scope and size in a second thread titled What Drawing Functionality Does SolidWorks Need to Improve?.  Finally, Mr. Livingston formalized the discussion under the thread SolidWorks Drawings ER Blitz, with the intent to finish compiling the list of requests by Sept 17, 2008.  By now, the list is over 40 individual items in about 15 categories.  Some of the categories are DRAWING EXPORT, DIMENSION, HOLE CALLOUTS, GD&T, and SYMBOLS.

Now, unofficially, I can say that SolidWorks Corp is aware of this list.  It is my impression that it will not be ignored.  That is not to say that every item will be dutifully explored and implemented right away.  There are many factors that go into decisions as to which improvements to work on first and when to implement them.  At the very least, SolidWorks Corp is listening.

Please check out the current list.  If so inclined, please feel free to voice your own thoughts about items on this list and mention any new items that need to be added.  What’s been bugging you?  What bugs need fixing? Where does SolidWorks not allow you to detail something per ASME or ISO standards without some heinous workaround?  Where is SolidWorks drawing functionality still lacking?  What functionality can be added to increase efficiency? 

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.