Category: Drawing

Product Review: Template Wizard (Part 2)

Template Wizard is a relatively new application from SolidWorks Templates by Kevin Van Liere.  He spent about 2 years developing and improving it.  It is designed to work within SolidWorks 2008, though it does have some limited functionality in SolidWorks 2007 SP4.0 or higher. This part of my article is a critique of Template Wizard’s specific functions and workflow.  Ultimately, the most important question will be answered “42”.  How easy is it to make a new Drawing Template with Template Wizard?

General Description and Workflow

This review is based on Template Wizard Version 2.5.3088.23714.  As stated before, Template Wizard allows for the creation of SolidWorks templates.  It is an add-in that runs from within SolidWorks.  When running, its interface occupies the Property Manager in what is commonly referred to as the FeatureManager or Feature Tree Pane, along the left side of the open document.  Settings and features are all selected from within this pane.

Once it is installed, Template Wizard appears as a pull down menu by the same name.  Two options appear in the menu.  “Create/Modify Templates” and “Help”.  This is very simple and to the point.  When selected, the Template Wizard pops up with some options to start a new template or modify an existing template.  These options apply to drawings, parts and assemblies.  However, if one selects anything other than Drawing Template first, the software gently reminds the user that it will work best if a Drawing Template is created first.

Template Wizard takes a step by step approach.  As one goes through the nine general steps for creating a Drawing Template, Template Wizard establishes its settings and allows the user to build what will become the Sheet Format and Drawing Template.  After that, it also flows right into the creation of part and assembly templates.  One minor drawback to this step-by-step approach is that the arrows which take you from step to step (backward and forward) are small and barely noticeable in the upper right corner of the pane.  The size of these arrow is controlled by SolidWorks itself (and not the fault of Template Wizard), but that doesn’t make it any easier to recognize.  However, once one is familiar with the interface, there are no usability issues due to this minor detail.

Creating a Drawing Template

Step 1 is the Template Wizards start-up form itself (where the user is wisely guided to first create a Drawing Template).  Once the choice is made and “Begin” is selected, a blank drawing is opened with Step 2 the Template Wizard appearing in the Program Manager.

Step 2 is very logical.  It requests sheet size, type of projection, unit system (in/mm, etc), dimensioning standard (ISO/ANSI, etc) and other fundamental settings.  As choices are made, they are immediately implemented.

Step 3 creates the border for the Sheet Format.  I’m not sure how much work went in to designing and programming this step (great or slight?), but in my opinion, this one step makes the whole Template Wizard package worth its price tag!  All the user has to do is set the margins, determine the number of zones and zone marker lengths; then click “Create Border”.  This step allows the user to generate a fully defined and complete border in seconds!  Advanced options also exist that establish other several settings.  The border can also be saved as a block for use elsewhere.

Step 4 allows the user to add title block elements to their template.  In my opinion, Step 4 is by far the most complex portion of Template Wizard.  It may even be a little scary at first.  There is a large selection of title block elements to choose from.  One must select each element from a drop down list box and place it on the drawing using the element’s insertion point.  It is fairly simply, but not immediately obvious, even with the on-screen description.  Before attempting to use step, I highly recommend reading the Help.  I especially recommend looking up “Pre-Designed Title Blocks” or “ASSY LOGO” in the Help to bring up images of the title block elements.  Once the user has the hang of how to pick and place the title block elements, this step easy and extremely powerful.  Template Wizard functionality does appear to be bumping into limitations of SolidWorks itself in this step.  One example of this is that if the user attempts to directly edit text within the template (instead of using Template Wizard functions to make such edits), SolidWorks will crash.  According to Kevin, this is a flaw in SolidWorks, but it is a flaw that pops up when using his application, so that may be a moot point.  I will say that if Template Wizard is used as intended, such issues should be minimal.

Step 5 directs the user to pick the Revision Table anchor.  Given SolidWorks 2008’s little quirks, I HIGHLY recommend choosing the upper right corner of the border.  It seems for some reason some functionality for creating Revision Tables has been reduced in 2008, making this necessary.  Very poor decision on the part of SolidWorks Corp., but I digress.  Template Wizard does insert the Revision Table once this anchor is selected.

Step 6 is a small step in which the user makes selections regarding fonts, annotations and display of tangent edges.  This step almost feels like an after-thought.  Perhaps these choices could be moved into Step 3 instead, or perhaps expanded to cover more settings that users may be interested in controlling?

Step 7 allows the user to save the drawing template (as it appears on screen) as a Sheet Format.  My only complaint here is that non-standard nomenclature is used.  Instead of referring to this function as “Save Sheet Format”, it has a button to “Save Page Design”.  I asked Kevin about this.  He made the choice to use this terminology because inexperienced users did not understand “Sheet Format” and how it is different from “Drawing Template”.  However, this choice may be confusing for experienced users.  Perhaps a statement in the on-screen help may allow Template Wizard to make this matter clear, especially if new terms are being created.

Step 8 is where the user actually saves their Drawing Template.

Step 9 allows the user to continue on to create templates for parts (models) and assemblies.  Template Wizard can carry over some information from the Drawing Template to these templates, such as unit settings and custom properties.  It also allows the user to control several other settings.  This function uses an intuitive and straightforward step-by-step approach to create those templates similar to how it works for drawings.

Conclusion

Template Wizard is a very well researched and useful product with a very low price tag.  Overall, it is easy to use and very comprehensive.  Kevin states, “I really put my heart into it to make it as good as I could.”  This dedication really shows in the end product.  The software is still a little rough around the edges in some places [as of 2008], though much of this seems to come from limitations or bugs within SolidWorks itself.  Given all factors, Template Wizard is well worth its price.  New and experienced users will benefit from this application.  Really, in my mind, the best customer for this software is anyone who has the responsibility to create templates for a new company or a company that has just started using SolidWorks.  The next best customer is one who wishes to improve already existing Drawing Templates.  I recommend Template Wizard for all such cases.

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.