Category: Drawing

Product Review: Template Wizard (Part 1)

One of the areas where SolidWorks lacks is in the creation and editing of engineering drawings.  Specifically, there is very poor support for drawing templates.  One person has taken a stab at filling this gap in SolidWorks functionality.  Kevin Van Liere of SolidWorks Templates has created Template Wizard.

The goal for Templates Wizard is to make it easy for the end user to create and edit drawing templates.  According to Kevin, SolidWorks Corp. does not acknowledge that their lack of functionality with drawing templates is a problem.  Also not provided by SolidWorks Corp. is a best practices guide for templates during SolidWorks training.  He developed Template Wizard due to these facts and out of pure frustration.

He says that his target is end users, of course.  In particular, new users will find Template Wizard most helpful, though he does feel existing users will benefit as well.  I am inclined to agree, especially at the current list price of {outdated}.  Due to the low price, he stated that some VARs have contacted him about purchasing seats of Template Wizard to provide it to their clients for free as part of an overall package.  For the price, this is likely one of the most accessible professional SolidWorks Add-ins available.

The Add-in creates templates for drawings, models and model assemblies.  It allows the user to create such templates from scratch. In the case of drawing templates, it also allows the user to create a SolidWorks drawing template based on an AutoCAD template.  Additionally, it will edit existing SolidWorks drawing templates to add fields and functions that might be previously lacking.

The focus is on the actual templates themselves.  For example, Template Wizard intentionally does not go deep in to settings, such as centermark sizes.  It does provide general control by the selection of ANSI, ISO, etc.  However, for the most part, it offers the pure experience of creating the template itself.  I think that task is daunting enough without getting into the numerous individual settings available within SolidWorks.

Part 2 of this article will go into the details of Template Wizard, focusing on its work flow and specific functions.  It will include a (hopefully) thorough critique of the Add-in.

For the record, this review is unsolicited by SolidWorks Templates; I contacted SolidWork Templates.  This review is based on a free short term license that was provided to me by SolidWorks Templates solely for the purpose of this review.  That license is revoked upon completion of this review.  No guarantees by me were granted to SolidWorks Templates regarding the outcome of this review.  I did discuss my negative findings with Kevin regarding specific functions prior to release of this review.  All of my findings (positive and negative) will be openly presented in Part 2.

Drill and Tap (~Part 3)

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

I previously discussed threaded hole callouts in the context of SolidWorks and its calloutformat.txt files (Part 1 and Part 2). As mentioned before, there is a tendency for some to callout threaded holes with too much information. Often, the thread callouts include the drill size. As argued before, including the drill size usually over-defines the threaded hole because the specifications of the thread itself identify the drill size. It also attempts to specify manufacturing processes, which is not allowed by ASME Y14.5M-1994. In fact, including the drill size within a thread callout may actually provide incorrect specification in many cases.

This is particularly true in the case of threads that are in blind holes. These are usually made with forming taps (roll taps). The diameter of the drilled hole for a roll tapped thread is bigger than it is for a cut thread. For example, for a 10-32 roll tap, the drill size is .1762, while a 10-32 cut thread drill size is .159. Once formed or cut, the specification for the ID of the thread is .156 to .164.

On drawings where customary units (inch) are used, the number of decimals places in the dimension usually determines the tolerance for that dimension. Stating a drill size as a decimal dimension applies the standard drawing tolerances to that dimension unless some general note is added.  This means that the tolerance for the drill callout likely differs with that required by the thread.  So, if the drill size is called out, drawing may be providing the wrong information to the machine shop.

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.

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.

How to use a Model’s Material directly on the Drawing

I should start out by saying that I personally advise against using the model’s Material value directly on a drawing (edit: for SolidWorks version 2008 and older; SW 2009 appears to have addressed some of the issues).  However, below is the instructions to do just this.

First, let me bring up three problems when it comes to materials and the SolidWorks Material Database naming convention.  One, the material names used in SolidWorks library are not correct.  In fact, in many cases they are not even the common names for those materials.  Two, for those of us who need accurate specification, the standards that define the materials are not mentioned of the library at all, making references to material incomplete.  Three, the names of the materials are not capitalized, so they are not formatted correctly to be used directly on a drawing in the first place.

A solution to these issues is to change your library to add this info and correct formatting or create a new library to do the same.   Another more common solution is to enter the information manually in a custom property within the model, then have that value pulled into the drawing via normal custom property linking, such as an annotation note with the following text: $PRPSHEET:”Material” or similar.  Make sure to identify which view you wish the data to be pulled from, within the Sheet Property window.

If you still wish to use the actual model’s material value (despite all of the above reasoning), there’s a couple extra steps (also involving the use of custom properties):

1.  In the model, create a custom property called something like Material at File>Properties>Custom tab.

2.   For the value of Material property, just click on the down arrow of the entry field and select Material.

3.  On the associated drawing, create similar custom property with the same name.  (Again, make sure to identify which view you wish the data to be pulled from, within the Sheet Property window.)

4.  For the value of the drawing’s Material custom property, type $PRP:”Material”

5.  Create an annotation note that links to the drawing’s Material custom property.  This will display the value of the model’s material directly on the drawing.

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.