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Change Your Life With SolidWorks "Search Options"

One of the great things about SolidWorks is that each new release is chock full of new functionality and improvements. The challenge of knowing where the settings are located that govern the behavior of all that functionality, unfortunately, becomes larger and larger.... until SolidWorks 2013.

In SolidWorks 2013, we have the same Options dialog that we've had in the past, with tabs and categories and all manner of controls, but we also now have a way to quickly find what we want -- it's called Search Options.

Say I'm working on a file from someone who didn't use the same document properties I want; maybe the arrows in sketches aren't to my liking. In the old days, I'd have to remember where those specific settings were located, or go through the Help and find it that way. In 2013, I can just type in the word "arrow" in Search Options, and immediately I'll have a list of each and every setting (both System Options and Document Properties included). What's more, I can click on that list and the Options dialog will jump to the described location for me, so I can literally click through and visually search for the page of settings that I want, with SolidWorks highlighting my keyword match on each page as I go:

Thus, on my third click in the list, I find the arrow settings I was looking for. Simple!

If you are a CAD administrator or a person who supports SolidWorks at your company, Search Options can make your life a whole lot easier. I won't leave home without it!

Safe Rollback in SolidWorks ePDM

There is a tool included with EPDM called Rollback.  This allows an administrator the option to delete current and previous versions to restore a file to an older version.  There is no control how far back the rollback allows a person to go so be careful who you give this to!  GXSC recommends only the build in administrator account be allowed the rollback option.  A person could rollback a released file to version 1, when it was an empty file.  It is best used as a tool to test new system changes on particular files, rolling back files as they go through states and transitions until the process works correctly.

Rollback is a tool found on the history of a file.  Simply click an earlier state and select Rollback.  The Warning:

Remember, be careful!  Those later versions will be gone forever!  

If the file you are rolling back is referenced you will get an error about that as well.

The result:

There is however a safe method to do a rollback, one that does not delete versions.  Any user can do this, granted they can "get" earlier versions.  To do this, check out the file and 'get' the earlier version:

Afterwards make your new changes, check in and write a comment about what you did.

Afterwards continue with the rest of your design process.  The next time it is approved to be released it will be the most recent revision, and not revision A or B.  In this case the next revision will be C.

A look at this history will show all is well.

SolidWorks, The Basics: Saving Sketch Dimensioning Styles

Can you imagine doing your job without the benefits of a top-flight 3D modeler like SolidWorks? I thought not. I am sure you remember the excitement you felt when you learned the power of the tool at your disposal. And the education didn’t stop there, did it? To this day, you enjoy learning new things. That’s why you’re reading the SolidNotes blog, right?  

However, here’s something I have long noticed: In my interactions with users, even very experienced ones, a lot of the questions involve seemingly basic procedures. I think it is easy to jump into the deep end and gloss over many such seemingly routine operations. Hence, another topic in my Basics Series: Sketch Dimension Styles.

We are often taught, when adding dimensions in a part sketch environment, to not worry about stylistic options or even exact unit precision or tolerances. That information can come later, on the drawing. That is often sufficient and is not incorrect. However, there are options that let you better tailor your dimensions in the sketch environment and can be instrumental in capturing intent and reducing errors downstream.

Fig. 1

Figure 1 shows the Sketch Dimension Property Manager. On the Value tab, we see a Tolerance/Precision node, under which I have selected Symmetric from among the many choices. Below that are pull-down menus that allow me to control the number of place precision of the dimension and its tolerance, and I have entered those tolerances accordingly.  

As this is something I plan to do with some frequency, I have chosen the “Add or Update a Style” and entered “3 PL” for a style name in the ensuing dialog box. I now have a named style that I may select to be current or use to change that of an existing dimension. As you might expect, these dimensions will keep these appearances when displayed in your drawing.

And…why, yes!   This *is* something I can create and save in my part template!  Similarly, this can also be saved as a style (“.sldstl” file format) and opened from another document, such as my drawing template, with the Load Style button.

 

Custom "Custom Properties"

Do you have custom properties that you use over and over in every SolidWorks part? It can get very annoying having to type those in over...and over...and over again! Many of you have probably noticed that in your Property Name field there is a drop down of a bunch of general property names.

Well, what if those aren't what your company uses on a regular basis? SolidWorks pulls those default items from a simple ".txt" file. It is easily edited in notepad to delete or add items on this list to suite your company's needs.

The location of this text file is set under System Option, File Locations, Custom Property Files

The default location of this folder is C:\ProgramData\SolidWorks\SolidWorks (Version)\lang\english

The location of this file can be anywhere as long as the File Location setting matches. This can be very convenient if you want this file on the network for everyone to use. The one catch is the file MUST be named "properties.txt"

So now to actually editing the file...open up the properties.txt file in notepad and you'll see a list of all the default property names. You can add, remove, or edit existing property names. The only requirement is that each property name be on a separate line.

Once the file has been modified how you want it, save it and you're done! Go ahead and start a new part and see your properties appear!

No longer will you need to go through the frustration of typing in your properties one at a time, every time!

 

ADDED BONUS!

Say all you want to do is quickly add a custom property to a large file that would take forever opening just to do a simple task...we've got you covered there as well!

In windows explorer, locate the file you want to add the custom property to, right click it, and go to Properties.

The windows file properties dialog box will be brought up. Under the "Custom" tab you'll see something that looks very similar to the File, Properties dialog in SolidWorks. Fill in the Name, Type, and Value fields and click "Add" and your custom property will automatically populate in your File, Properties within SolidWorks!

 

 

I Knew It Was Somewhere...

For those who have taken my Advanced part and Surface modeling classes, you know that one of my favorite ways to inspect curvature is to use curvature combs. These are graphical elements that display the amount of curvature at a given point on a sketch element. They’re fantastic for predicting problem areas in sketches, especially splines, that will be used to generate complex surfaces.

To display curvature combs for a sketch entity, simply right-click on the entity and choose Show Curvature Combs from the pop-up menu. When you do, SolidWorks will create a set of lines normal to the sketch entity at points along that entity; the longer the line of the comb, the more curvature there is at that point.

While the combs are very useful as is, they become even better more useful when you turn on the bounding curve. The bounding curve of a curvature comb makes it very easy to see even subtle changes or inflections in the curvature of an entity.

 

Curvature Combs with Bounding Curve off

 

Curvature Comb with Bounding Curve on

 

To turn on these helpful bounding curves, go to Tools, Options, System Options, and pick the Sketch page. On that page you’ll find a checkbox: Show curvature comb bounding curve.

 

It’s an option I knew I had, but I had forgotten about it until recently when I was trying to explain using Curvature Combs in an Advanced Part class. I could mentally trace the flow of the curve because I knew what I was looking at; my students had a harder time until I increased the density of the curvature combs. I then thought to myself, “Wasn’t there a way to show the flow of these curvature comb ends?” A little digging into the SolidWorks option pages and there it was! Use it and you’ll find it even easier to predict surface behaviors when created from your sketches.

Balloons and Excluding From Bills of Materials

I recently took a support call from a customer who noticed that he was seeing asterisks instead of item numbers when he added balloons to a purchased sub-assembly inside of his assembly drawing. I thought that it might make for a good case study about what caused the asterisks to show instead of item numbers, and what alternative methods could be used to achieve the customer's desired result.

As an example, let's suppose that you manufacture toy foam arrow guns, like the one below:

The toy consists of a main body sub-assembly (SUB_body.sldasm), two copies of a sub-assembly for the "trigger" (SUB_trigger.sldasm) and two copies of a part that defines the foam arrow (Arrow.sldprt). The different components are highlighted in the color coded image above, and you can see the full tree structure of the assembly to the left (click to view in a pop-out window).

As in my support case, let's suppose that one of the sub-assemblies (SUB_body) is a purchased component, and that your purchasing department will not need any details from the sub-assembly components (Finger Grip, Nozzle, and Main Body). In that case, you wouldn't want or need for those components to show up if you did a detailed bill of material in your drawing for the top level assembly.

How do you go about doing this? If you're like the customer that called into me, you would go into the component properties for each component within SUB_body.sldasm, and select the "exclude from Bill of Materials" option and go about your business.

However, if you create an indented or parts-only BOM on your assembly drawing, you will see this when you add your balloons:

Notice how the balloon coming off of the fingergaurd on the body sub-assembly has an asterisk instead of showing item #1. The reason this happens is because the balloon leader is attached to physical geometry- in this case, an edge that belongs to the finger grip part. Since that part has the "Exclude from bill of materials" box checked, it does not get an item number assigned to it, and the balloon field defaults to show an asterisk instead.

If you want to see a real item number show up in that balloon, you have a few options to work around this issue:

1. Use a Top Level Only bill of material, which will remove your ability to call out the trigger sub-assembly components independently.
2. Attach the end of your leader to an assembly feature within SUB_body.sldasm. You could select the origin, or an assembly feature (such as a sketch).
3. If you truly do not care about the sub-components in your assembly, you can save the assembly as a part file.
4. Clear the "exclude from Bill of Material" option in all of your subcomponents. Go to the configuration options within SUB_body.sldasm and look at the Bill of Materials Options. You will see an option for "Child component display when used as a subassembly". Switch from the default "Show" option and select "Hide".
   
   "Hide" will perform the same task as excluding all of your subcomponents, but it will also help you keep your balloons simple. Now, when you select an edge or surface from the Finger Grip, Nozzle or Main Body components, the balloon will grab the item number for the subassembly, instead of defaulting to the asterisk. The "Promote" option would remove the subassembly from the bill of material, and promote all of the subcomponents in its place.

Here is an example of what that drawing would look like if you elect to go with option 4:

Set Default SolidWorks Version for Opening a File

If you're like me, you have more than one version of SolidWorks loaded on your computer. Most of the time, I launch the version of SolidWorks I want to run, and then open my files from inside the application. But sometimes, I just double-click on a file and have Solidworks launch that way. There isn't anything inherently wrong with this; however, if you don't want to bring the file into the latest version of SolidWorks, you can be frustrated.

How Do I Handle This?

When you double-click on a file, you expect an application to launch and then load the file for you. But how does Windows know to open an .sldprt file in SolidWorks and not Notepad? Windows looks at the file extension and uses "file association" to figure it out.

File association is nothing more than a lookup in Windows: if the extension is .docx, open it in winword.exe; if it's .txt, open it in notepad.exe. These associations are defined when you install applications. If you install a later version of an existing application, the association for the related file extensions will be changed to the newest version of the software program.

I Don't Want The Newest

So, what if you're participating in the SolidWorks Beta program? In that case, users generally want to make sure that when you double-click on a .sldprt file, it opens with SolidWorks 2012 and not Beta 2013. Likewise, if you are working on a project collaborating with others using SolidWorks 2011, you don't want to absent-mindedly double-click on a file and accidentally bring it up in 2012. Can you tell Windows to use an older version of SolidWorks as the default program for File Associations? Yes, and it's easy.

Right-click on an example file of the type you're trying to set (such as a SolidWorks part file) and choose "Open With..." from the resulting popup menu. What you want to do is go to the bottom of the resulting list of programs, and click on "Choose Default Program..."

Once you do that, you will be brought into a dialog box to choose what program to use with this type of file:

Notice that only the latest version of any application will be shown in that dialog box. If you want to choose an older version of sldworks.exe, for example, you'll need to Browse... to it. In the example below, I'm going to choose SolidWorks 2011:

Once that's done, the association will be made. Note that while it's possible to make the new association specific to the file you've right-clicked on, the default behavior is to make this association change with all files of that particular extension (in this case, all .sldprt files).

Note that this technique works with any files and any programs on Windows. So, if you want to open up .jpg files in Windows Live Photo Gallery instead of Windows Picture Viewer, you can use this to take control of what happens when you double-click that digital photo.

 

Command Search: What's Old Is New

Remember in ancient times, when you used a DOS prompt? Perhaps your command environment of choice was -sh on a Unix system, or maybe you rocked the $ prompt in VAX/VMS. In any case, you probably made good use of command search paths and aliases. In those days, you had command-line interaction and nothing else -- some people even liked it.

Fast-forward to the 21st century, where icon-driven interfaces are clicked with a mouse or touched with a finger. Even in this environment, the ability to type in a command is desirable: the more icons you have, the more desirable it is.

Thus, we find command search (or actually, pervasive search that includes commands) implemented in Mac OS, Windows, iOS, and Android. It's very convenient to go to the Start Menu in Windows and type "Printers" to get directly to that area of the Control Panel.  For example, I find the reason most people don't use it is because they don't know about it. The only more convenient thing would be for my device to carry out commands by voice (which is already there on some platforms, in varying modes of reliability).

So it comes to pass that SolidWorks has command search in the latest incarnation -- SolidWorks 2012. You can click on it in the regular search window (it's the one with the >_ icon) or, more conveniently, it's automatically activated and given keyboard focus every time you hit the S key (you DO use the S key for your custom shortcut menu, don't you?)

You can type in part of a command (try "hole" if you're in a part) and you'll get a number of matches. Hit "Enter" and the top match will execute, or click on another item in the list to do that command instead (arrow keys work in the list too). If you want to drag it into the Command Manager, you just rip it right out of the list. Or use the eyeglasses icon to the right of the command in the list to see where it is in your existing interface.

If you want, you can make your own "shortcuts" to commands you use often. Think of these as nicknames. I've nicknamed "Hole Alignment" as "ha" so if I type in "ha" it comes to the top of the list; an Enter key later and I'm using the command I want. You can make these in the Customize interface (there is a new column called "Search Shortcut").

Once you try Command Search, I think you'll really like it. And if you haven't tried it in Windows or on your Mac or your smartphone, give that a shot too. Before too long, I believe you'll be speaking commands to your computer but in the meantime, What's Old Is New.

Alternate Mode for Running Commands in SolidWorks

SolidWorks commands are usually "sticky": they continue to run until you turn them off. For example, if you choose to create a rectangle, SolidWorks keeps you in the rectangle command until you either click the button again to toggle it off or hit the Esc key.

If you would prefer that a command only run once, then turn itself off (automatically putting you back into the "arrow" or Select tool), turn on the option "Single command per pick" under Tools, Options, System Options, General:

Now, when you choose to run a command, that command will run only once. If you decide you want a command to "stick", you can accomplish that by double-clicking the command button instead of single-clicking.

When an Rx Won't Capture It

SolidWork's Rx utility is a great tool for logging repeatable issues such as crashes or errors.  While it works well with SolidWorks, what happens when you are using eDrawings, the 2D Editor, or Draft Sight?  I'd like you to consider some free and internal tools to help you log repeatable issues.  This will help your and your VAR in troubleshooting the issue and finding a solution.

The first is a free download from www.sysinternals.com or Microsoft.  Process Monitor allows you to quickly create a capture filter for a particular process (such as sldworks.exe) and see, in real-time, what registry and system calls are being made.  While cryptic at times, the technical support staff at your reseller and at SolidWorks corporate can use the logs saved to learn more about the process' behavior.  Warning: log files can become very large depending on how long you log for.

To create a filter, use the short-cut (CTL-L) or drop down.  The window looks like this:

You can see above that I've created a filter for the eDrawings executable.  A screen shot of a running filter looks like this.

Now I can see what the process is doing, what keys its touching, and if there were any failures.

To go a step deeper, you use the built-in Event Viewer.  In Windows 7, right from the search box you can simply type "Event Viewer" and select it to launch.  It looks like this and is comprised of logs for applications and system events.

Expand "Windows Logs" and select Application or System. Scroll through the log at top and look for warnings or errors.  These are the same logs captured with an Rx.  But, again, what do you do with eDrawings or Draft Sight? (or AutoCAD, or ProE, or .... you name the application)

Here are examples of App events and System events.

I hope you found this blog useful.  The next time you get an error or warning, now you may have one more tool in your belt to use to troubleshoot.