Graphics Systems SolidNotes

Optical Illusion - Or Not? A SolidWorks Modeling Challenge

As designers, we are always encouraged to see things from a different angle. To think outside the box, as it were, to use both sides of our brain. Visualize a solution to a problem and then plot the steps toward its solution. But whether you are naturally left- or right-brained – hey, we all need a break once in a while!

So, I thought I’d start off the New Year with a light-hearted challenge: Can you model this in SolidWorks?

Is it just an optical illusion? A creative use of Planes during model creation? Some Photoshop trickery? All of the above? Use the Comment fields below to give us your ideas . Hints (besides the one already included), if not the final answer, will be given in an upcoming post.

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New To SolidWorks? – Sketching Tips II

First of all: Thank you.

Thank you for attending our recent annual GXSC User Conference and making it the premier event of its type for SolidWorks users. We loved meeting our customers and hearing their success stories.

But I really came to talk about more sketching tips. If you read my post from last month, you know I have a leftover problem. I bit off more than I could chew when creating my presentation and had to pare back a bit. One of the tips that did not make the cut was: Did you know you can use the Power Trim command…to extend objects?

That’s right! You are used to starting the Trim Entities function, double-checking that the Power Trim button is engaged, and then simply holding down the left mouse button and swiping across objects to trim them. Next time you need to extend objects until they intersect another, try the same approach – but hold down the Shift key while swiping. Voila! On a similar note, have you ever noticed you can right-click while in either the Trim or Extend command and toggle to the other from the context menu?

My other tip today is in answer to a question I received at our conference: After using the Select Contour Tool to denote some number of regions for feature creation, is it possible to edit that afterwards? The answer, of course, is…yes! Using whatever method you prefer, start the Edit Feature function on the object in question. The key is to highlight the Selected Contours field in the Feature Manager before selecting new regions. As shown below, you can also right-click on a region to deselect it.

 

 

New To Solidworks? - Using Text In Sketches

Leftovers. Some say they’re the best part of a meal, but how do we make sure they don’t go to waste?

I was recently faced with that exact problem. I cooked up so many topics for my SolidWorks Sketching Tips presentation at the upcoming annual Graphics Systems’ User Conference (you are attending…right?), that I just plain ran out of time to include everything I’d hoped. Not one to let a juicy tidbit go to waste, I thought I’d give everyone something to snack on. It’s easy to digest…and it’s pretty sweet!

It’s a pretty straightforward recipe, really. After starting a sketch and selecting the Text tool from the Command Manager, simply select a model edge or sketched object for the text to follow. TIP: If using a sketched object, make sure to first turn it into Construction Geometry by selecting the object and then the appropriate tool from the context menu, as shown below.

If you’re a routine user of any text editing software, you’ll probably recognize the formatting options presented in the Sketch Text command. Of particular interest, though, are the “Link to Property” and “Rotate” buttons in the upper left and right corners, respectively. (Link to Property – just think how powerful that can be for embossed/engraved part numbers or other product data.)

 

Another tip: The text height can be controlled either through the document font settings or through the standard Windows font selection tool if another is specified.

As mentioned, text can easily be placed along a model edge:

If you’re hungry for more tasty tips, make sure to attend our annual Graphics Systems’ User Conference.

Use the Indent Command for That!

One of my go-to SolidWorks modeling features is Indent. When it was first introduced, it was touted as a way to "impress" one model into another -- like putting your thumb into a hunk of wet clay.

More often, however, I use the Indent command to take one part and cut out material from an overlapping part. This is accomplished by the small "Cut" option in the Indent command. That option, "Indent as Cut," makes the command much more versatile. This is also more useful to the average SolidWorks user.

It's easier to show examples than to explain; so, I'll end the up-font commentary by saying Indent is one of the few commands I've actually added to my Features Command Manager. It's very useful as it works with multi-body parts and parts in assemblies as well.

This is the way people normally think of using the Indent command. Notice you can determine the side of the extra material by what you click on in the graphics window and the corresponding "keep/remove selection" setting in the command.

Here's an example of a "normal" Indent:

This is the result of the Indent command with the settings and model shown:

Now, if you modify the Indent command by turning on the "Cut" option, the behavior changes. Remember, this is just calculating geometry so it doesn't matter if the parts are shelled or not:

So you can see the results of the Indent command with the Cut option turned on. Think of the time savings for all kinds of models -- I see a lot of people copying sketches or making their own offset sketch geometry to achive associative holes and cutouts for other bodies or parts. Indent with Cut does it for you much faster, easier, and more robustly!

If you have an open part (think tube or hollow shaft) the regular Indent command works to build material around the end:

But if you use the Indent with the Cut option turned on, you get a hole! Note that the center core will also be there as an extra body, which is sometimes useful but more often than not you'll just suppress or delete it.

The Indent command is one of the most useful features in my SolidWorks toolkit, yet I almost never see it used. It's not just for consumer product designers -- it's for packaging design, case goods and furniture, tool design, and machine design. It can do lots of jobs better than older 3D tools and sketch-based methods, yet is seems people just don't know about it. So please share this article and spread the word: "You should use the Indent command for that!"

Design Inspiration - And Other Tools of the Trade

The goal of our SolidNotes blog and training classes is simple: to help you learn more about the tools of your trade.

Hopefully, we've been successful and you have discovered some new, unique software tips and tricks. Perhaps you've gained knowledge about workflows and therefore improved your efficiency. Maybe we've even been able to help your company reduce costs or time to market by helping best utilize the file management, prototyping and simulation tools available to you in SolidWorks.

But have we made you a better designer?

In a quest to continually improve myself and skills, I have always sought out resources such as this SolidNotes blog. But in my search for information, I have always tried to devote part of that time to inspiration. And there are not many designers who I’ve found more fascinating than Brooks Stevens.

Brooks has been described as “a functionalist but also an aesthete” although he more humbly describes himself as a “businessman-engineer and stylist.” He is known for coining the term, "planned obsolescence.” What most impresses me about his designs and those of his firm, are the sheer depth and breadth of industries and disciplines they span: industrial and product design, facilities and architectural design, packaging, appliances, marketing collateral, lawn and garden, and many vehicular designs – from Studebakers, Harley-Davidsons, Willys and Cadillacs to…yes, the Oscar Mayer Weinermobile!

Perhaps my favorite story involves his responsibility for increasing sales of clothes dryers by changing not the fundamental design, but…adding a window so consumers could see the  machine in action. This is exactly the kind of inspired thinking that has driven my love for designers and their tools.

 

If I’ve piqued your interest, much more information can be found at the Wisconsin Historical Society, the Brooks Stevens History website, and of course Wikipedia.

So please, spend some time reading through our blog, and check back often. We know there are many things we can teach you. And maybe, if we’re successful, we just might inspire you as well.

New To SolidWorks? Get your Sketching Grid Back!

Are you a recent convert to SolidWorks, despite having used other similar programs? You may have had many preferred settings you now wish to replicate in SolidWorks. One such function may be the appearance of a grid while in the Sketch environment. Sure, there are other visual cues that indicate you’re editing a sketch, such as the appearance of the appropriate icons in both the Command Manager and Confirmation Corner (see Figs. 1 and 2), and over time you may find these indicators suffice.

 Figure 1       Figure 2

However, it is possible to display and utilize a grid while sketching. First, invoke the Options dialog box through either the Options pull-down (Fig. 3) or Tools pull-down menu (if enabled).

 Figure 3

Select the Document Properties tab and then the Grid/Snap node from the left-hand column (see Fig. 4). It is here that you will find the option for turning on the grid as well as other appearance settings.

 Figure 4

It is important to note that you’ve made these changes in your local Document Settings – if you want all new documents to default to this behavior, then this setting may be best made in your part templates.

 Figure 5

In Fig. 5 we see a reflection of the above settings.  There is no “best” setting – experiment and find what works best for you.

2011 Graphics Systems User Conference Announced: Call for Presenters!

Become Part of the Largest SolidWorks Conference in the Midwest!

Graphics Systems Corporation's User Conference is back for 2011 and it will feature more in-depth training sessions and new engineering technology than ever before.  Currently we are looking for SolidWorks engineers to help us shape the conference's content to focus on the issues you think are the most important.  

Make your voice heard and help your fellow SolidWorks engineers by suggesting or voting for session topics or applying to present a topic or case study!

Suggest and Vote for the Topics you Want!

The Graphics Systems User Conference is the only place in the Midwest where you can pick from several unique tracks including: SolidWorks Design, Simulation, Data Management, Technical Communications, and Management.

The conference agenda is determined by you! You can help shape the topics covered, by suggesting and voting on the topics you want to see. The most popular topics will be placed on our agenda when it is announced in August 2011.

>> Suggest & Vote For Topics Now!

Become a Presenter!

• Want to share your SolidWorks expertise with fellow engineers? 
• Do you have an innovative product you've designed in SolidWorks that you'd like to share/promote?

If so, you should apply to be a presenter or customer success story at this year's GXSC User Conference!  Selected presenters will receive a complimentary hotel room and conference pass.

>> E-mail Us with your topic idea and we will contact you very shortly.

To learn more about the 2011 Graphics Systems User Conference, visit the event website today!

Modeling Twisted Parts

Sometimes it's necessary to model things we ordinarily wouldn't in SolidWorks. Take twisted parts, for example. If you had a cable in your assembly that was made up of several smaller strands twisted together, normally you would just model the cable as a sweep with a single circular profile. But what if you MAKE those cables? Can you actually model that look for use in a drawing view or a rendering?

Yes, you can.

There are a few methods that can be used to do this, but the easiest one is a single swept profile that has multiple contours. You can use this in combination with the "Twist" option in the sweep, and by specifying by "Turns" you can easily get a look to convey what you want:

This works because the sketch has space in between the contours, resulting in multiple bodies:

 
 
Note that using the Twist is going to twist the sketch around the centerline as the sweep progresses. By definition, this is going to narrow the resulting geometry, and it won't be perfectly round in a cross-section perpendicular to the sweep path. For coarser twists, this is barely noticable.

 

At 20 turns, the effect can be more easily seen, but for visual representation it works fine and is still not very pronounced:

 

The tighter twists are going to start to show more pronounced distortion, which may or may not be acceptable, depending on your application:

 

It would not be possible in "real life" to have 50 turns of that thick of material; it would intersect itself geometrically. Which is why this technique tends to fill the bill for most people looking to show this in a model -- the number of turns fall closer to the first example than the last.

Change to Toolbox References in SolidWorks 2011

In SolidWorks 2011, there is a new option in Tools > Options > System Options > Hole Wizard/Toolbox. I've taken a screenshot and highlighted the new option in yellow:

This option didn't exist prior to SolidWorks 2011, and for some people it can be a Good Thing. What it does is tell SolidWorks that whenever it finds a reference to a Toolbox part, go to this one specific folder to find the corresponding model. If you have mistakenly referenced Toolbox files from different locations, this can be an easy way to get things referenced correctly.

However, there can be a down side. IF you use Toolbox as a "part generator" to create your own library parts, then doctor them up and store them in another location (such as a regular Design Library folder on your network), this can cause a problem. You see, even though you have referenced the "custom" parts from your external library folder in your assemblies, the parts are still Toolbox parts. Also, if this new option is turned on, the next time you load your assembly, it will get the original Toolbox parts from the original Toolbox repository.

So, big deal -- don't turn on the new option. Then Toolbox will behave just as it did before 2011, right? That is correct, but the wrinkle here is that the new option is turned on by default. Since it didn't exist before 2011, there is no "old setting" to copy, so bottom line is this new option -- and this new Toolbox behavior -- is turned on for everyone in SolidWorks 2011 whether you want it or not. Not a big deal, since now you're aware of it -- it's a one-click fix. But if you missed it in the What's New, it can cause a little head-scratching. Until now, because I've just explained it to you :)

Changing the Fixed Face for a Sheet Metal Flat Pattern

I get questions from time to time regarding sheet metal flat patterns, specifically, "How do I change the 'up' side of a flat pattern?"

Sometimes you just want to change the direction of a flat pattern, i.e make "up" be "down." One way to do this in SolidWorks 2011 is to simply select the flat pattern drawing view, look at the properties of the view, and click on a button to "Flip view," as illustrated:

 

If you want to take this a bit further, besides simply reversing "up" and "down," you can open the SolidWorks sheet metal model and directly select any face in the model to be the "Fixed face," which is the face that is "up" when SolidWorks generates a flat pattern.

To do this, edit the Flat Pattern feature and select the top box, labeled "Fixed face." Next, select any face in the model. This face becomes the new "top" for the flat pattern, as well as the face other faces unfold flat to, as shown:

Here is an example of what would happen if you picked a different face as the fixed face in the same model:

As you can see, you have the ability to make any face the "up side" of a flat pattern, giving you total control of the flat. If we could only control the weather like this, we could avoid April snowstorms like we had last week!