I have often been asked about coordinate systems when it comes to CAM vs.CAD. In a nutshell, CAD systems like SOLIDWORKS and CAM systems use different directions for defining coordinate systems, specifically in regards to Y and Z. The result is, when a model is exported from SOLIDWORKS and imported to a CAM system, the model comes up in the CAM system in the "wrong" orientation. The good news is a SOLIDWORKS user can make their own coordinate system specifically for use in the export process, thus resulting in a model coming up in the correct orientation in the CAM program.

The first step is to make your new coordinate system. Click on the "Reference Geometry" button on the Features tab of the Command Manager:

Next, select a point on the model or use the Origin of the model to define the origin of the new coordinate system:

Now select edges to define any two of the X, Y, and Z axes for your coordinate system. Use the double-arrow buttons if you need to reverse positive direction. In my case, I'm picking edges on the model to define X and Z as shown:

The final result is a new coordinate system. Notice the direction of X, Y, and Z in the new coordinate system vs. the standard coordinate system.

To export the model using the new coordinate system, do a Save As, choose your file type, click the Options button, and make sure you change the coordinate system from "Default" to your new coordinate system near the bottom of the dialog box.

And, that's it! Now you can save out any SOLIDWORKS file to any coordinate system you can define.

     

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By: John Setzer, Training Coordinator

Enhancements in SOLIDWORKS 2016 make picking similar components in an assembly a snap! Just use the new "Select Identical Components" command found in the Selection tool fly out:

Getting Started

Once you start the tool, there's an option in the Property Manager to Match configuration names. If this is checked, then only components with the same name AND same configuration will be selected.

In the example below, we have three instances of a part named pin_&. When Select Identical Components is run with Match configuration names active, selecting one of the SHORT pins will result in the two SHORT pins being selected, but not the LONG pin.

If you clear "Match configuration names," you will get a different behavior. Instead, all components of the same name will be picked regardless of configuration, so all pins will be selected.

Note: if you pre-select a part you won't get the Property Manager. Instead, SOLIDWORKS will use the last setting used for the Match configuration names option. I find this command extremely handy and I have customized my system so the Selection tool flyout is on my pop-up toolbars. (Remember, you can customize these as of SOLIDWORKS 2015!)

To add this button to your pop-up toolbar, select a component in an assembly to bring up the pop-up, then right-click on the pop-up and choose "Customize." From there you can go to the Standard page under the Commands tab, and drag and drop the Selection Flyout tool onto your pop-up toolbar. Now, this handy new command will always be at your fingertips when you select a part in an assembly!

     

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By Marty Bucholz, Technical Support Representative

In SOLIDWORKS 2016, there's a new feature called instant 2D that allows for immediate direct editing of sketch dimensions without having to rebuild to reset the geometry. More importantly, it changes how you interact with dimension values. With instant 2D enabled, you can still move your dimensions and adjust their placement by clicking on the leader lines, not the dimension number itself, which can take a little getting used to. First, let’s understand the tool's benefit.

The most obvious benefit of this tool is that it allows you to single-click on dimensions to edit the value of the dimension. 

Additionally, once you have clicked on the dimension you can grab the dimension handles and drag the sketch and dimension out to edit it.

Both of these methods of rapidly changing sketch geometry while keeping it dimensionally controlled can be a very powerful tool in your design process, especially in the early stages.

With some small or hard to place dimensions, you may still want to disable this feature to get your dimensions in just the right place. Instant 2D is located on your command manager in the sketch tab at the end of the ribbon. Toggle it on and off as needed to while using Solidworks.

     

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For many of us, SOLIDWORKS PDM proves to be a lifesaver in automation time and again. To make data entry a lot less painful and more practical, there are a few things we can do on the front end. I was reminded of this during a recent encounter dealing with variable names.

The Problem

In this specific instance, there was a field within the drawing that needed to be driven by a data card variable. A company had multiple locations with different company identities at each location. If the location was set to "City A" on the data card, then the drawing needed to show "Company A" in the title block. This can be achieved rather easily with the following steps.

First, a few things to consider with this method and example:

• It is assumed PDM variables have been created and the drawing property has been appropriately mapped. Variable mapping is discussed in greater detail here. In this example, I used the variable names TEST_Company and TEST_City.
• This is not a two-way interaction, so one property must drive the other. In this example, TEST_City will drive TEST_Company.

Now to the good stuff, here's how to define the relation between the two properties:

1. Once the variables have been created and appropriately mapped on our drawing property, we must define a list. We'll do this in the PDM Administration tool (Start Menu >> All Programs >> SOLIDWORKS PDM >> Administration).
2. With the PDM Administration tool open, we will need to log into the vault and expand the vault node.
3. Then right-click on Lists (for cards) and select Add New.
   
   
4. In the List dialog, select Text With Alias as the data type and enter a preferred list name.
   
5. Populate the list with Displayed Values/Cities and a corresponding number starting at 1, as shown above.
6. Navigate to File >> Save to complete the list creation.

It's now time to make our data card modifications. Open the Data Card for these properties and start the setup process. In this case, the properties are entered into the part and carried into the drawing, which means we must edit the part card using an edit-box for the controlled value and a drop list for the controlling value.

We'll start by creating an edit-box that links to TEST_Company, followed by a drop list that links to TEST_City.

Next, we will need to configure our edit-box and drop list.

For our drop list, we must change the following parameters:

• Items: Special Value - Alias List

For our edit-box, we will change the following parameters:

• Read-Only: Checked (Because city is the driving factor, we don't want to allow direct edits.)
• Default Value: Text Value
• Input Formula: See Below.

Finally, we must define an input formula for our edit-box using the $Token command. The syntax for this command is defined as:

$Token(|||,,|)

- List of strings to choose from.

- Index of strings to use. This could be a variable linked to an alias list.

| - The character used to separate the values.

For example:

$Token(Company A|Company B|Company C|Company D|Company E|Company F,%TEST_City%,|)

The above command basically states if the alias of TEST_City (as we defined when we created the list) is 1, then the value will equal Company A. If it is equal to 2, then the value will be Company B, and so on. Once the defined formula syntax is inputted, the value of TEST_City on the data card TEST_Company will populate automatically when changed.

This is a great way to use the built-in capabilities of SOLIDWORKS PDM to enable functionality that is otherwise difficult to achieve. The time savings and reduced data entry for users is always a good thing.

Happy Vaulting! 

     

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By: Evan Stanek, Electrical Applications Engineer

As a child of the '80s, I’ll always remember the first time I saw MacGyver get out of a jam using the most elementary of tools he found in his surroundings (diffusing a bomb with a paperclip, please!). I'm sure his adventures were the inspiration for many careers in creative problem solving for profit (e.g., engineering). Our day-to-day work doesn’t quite have the same sizzle - drawing schematics just doesn't have the same appeal for TV. However, SOLIDWORKS Electrical Connection Labels may just make you feel a little more like MacGyver, that is if he had access to the luxury of a Swiss Army knife instead of a wad of ABC gum and a paper clip.

Connection labels are completely customizable symbols that show a miniature “to/from” report for any component. The labels can appear as a simple table with rows and columns or as a display of the information with supporting graphics matching terminals and ins and outs to a real part footprint. Connection labels have the ability to call on information and display it in any part of your design (e.g., line diagrams, schematics, reports, 2D layouts, etc.), making it a pretty versatile tool. Hence, the Swiss Army knife comparison!

Once you've populated the rest of your library and have thoroughly defined your schematics, you can then get to the fun part of retrieving "the good stuff." Just like reports, connection labels are perfect for retrieving the information you’ve already built into your parts and design.

There are two types of labels, blue and red. Blue represents the circuit information (to/from, wire/cable info, terminals) of a manufacturer part in your design.

These can be directly mapped as a default within the manufacturer parts properties! 

The red connection labels represent detailed information based on the top level component in your design (multiple parts apply!). 

There is a host of attributes available for display, and the label will instantly update the information for which they point to reflect changes in other parts of the design. Some labels are packaged by default in SOLIDWORKS Electrical, but you can also take a crack at customizing options to fit your needs.

You can always create a new label just as you would for any other symbol (be sure to select “Connection Label” in the symbol type drop-down). Or, make a copy of an existing label and save time using the copied attributes instead of clicking to insert your own.


Of course, we can display the usual information (e.g., component mark, manufacturer, descriptions, reference number), but further down in “Connection Point” is where the REALLY good stuff lives. 

From terminal mark and mnemonic information to wire and cable assignments to wire cross sections to cable cores and properties and much more, all are at the ready and can be called upon using the corresponding attributes. When selecting your attributes, SOLIDWORKS Electrical will ask you which circuit you want to use for the labels and will apply the proper circuit tag accordingly!

Since the majority of the symbol work for connection labels deals with attributes, here are a few helpful tips to make connection labels more efficiently.

• Make your largest connection label first (most terminals needed), then copy/paste the attributes you’ve chosen for all other smaller labels to avoid re-inserting/renumbering.
• Use of left > right vs. right > left dragging to select only the parts of your symbol that you're working on.
• If a table or generic symbol is sufficient, reuse the same connection label for many types of components to get the point-to-point information you want.
• Make use of “copy properties” and “apply copied properties” to make all your attributes match in style, justification, and size.
• Remember, you won’t need to add connection points, those are only needed for multi-wire symbols!
• Use the "array" and "multiple copy" commands to quickly and evenly place lines and text when placing grid lines or copying attributes.

Don’t hesitate to try it out and experiment to see how it fits into your engineering process.

     

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By: Sam Hochberg, CSWE, Applications Engineer

It has been a couple of weeks since we last checked in with our resident SOLIDWORKS swami, Sol, and his somewhat simpler sidekick, Sal. After their recent professional skirmishes, I'm sure we're all curious to see what they’re up to now…

“Hey Sol, not bad, eh?” Sal said, smiling and motioning toward his computer screen.

“Yes, not bad,” Sol said, looking at Figure 1.

Fig. 1

“Not bad at all for my first SOLIDWORKS Composer job!" said Sal. "It was just as easy as you said it would be and I like easy!”

Sol sighed and shot Sal a sideways glance, but subsequently softened. “Hey, I have a neat trick for you. Have you thought about creating different appearances on different parts?”

“Like one part shaded, another not...like that?" Sal asked. "But, how do I do that? All I saw was one overall selection!"

“Well Sal, remember that individual actors have properties just like the entire scene does,” Sol said. 

Sal’s eyes sparkled with excitement, “Are you saying that…”

Sol sensed Sal’s steps toward sentience. “Yes, Sal. Here’s how you do it," Sol continued. "First, we have to select ‘Custom’ as our Render Mode. Take a look down there at Figure 2.”

Fig. 2

“Now you’ll see that after selecting an actor, such as the car body, it has its own Rendering options. See down there in Figure 3?” Sol explained. 

Fig. 3

“Sure do, Sol!” Sal said. Sensing something stupendous was soon to be seen, he started salivating like Pavlov’s own dog.

“Go click where it says ‘Smooth’ and see the other options in the pull-down menu," Sol said. "I suggest selecting ‘Silhouette’ for the car body!”

“Well, I’ll be…” said Sal, looking down at Figure 4, “You can see all the stuff inside!”

Fig. 4

“Don’t make a scene, Sal,” Sol teased.

“What?” Sal asked. 

“It was a rendering joke, Sal. Get it?” Sol laughed. 

“Nice! Remind me, Sol, where do you get all of this fantastic SOLIDWORKS information?” Sal inquired.

“Why, Graphics Systems’ SolidNotes blog, Sal. Graphics Systems’ SolidNotes.”

You can see several more of Sam’s somewhat serious series of Sol and Sal’s serial spree of SOLIDWORKS shenanigans here and here and here and here…

     

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Last week we got an interesting question that I thought I'd share with you. A customer was wondering if there was a way to have SOLIDWORKS tell him where he needed to hang a beam from so that it would hang at a specified angle when picked up by a crane. We put on our thinking caps for this one. We probably could've used some simulation tools like SOLIDWORKS Simulation or SOLIDWORKS Motion to solve this problem, but ultimately the best solution, in this case, was a good old hand calculation. I had to reach way back into my statics knowledge to solve this. All this problem is a Sum of Moments problem. Summing the moments about the point we want to hang the beam from lets us get an equation where the only unknown we have is the distance we're looking for. The free body diagram and equation looks something like this.

This got me thinking, though, why not do this in SOLIDWORKS? That way it can be used for whatever size beam! All we have to do is create a couple variables and link them to model dimensions and input this big long moments equation and we're done! Check out below how I did this and feel free to utilize this for something similar you may run into!


By: Chris Olson, Simulation Applications Engineer

     

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