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Posts Tagged ‘SolidWorks 2008’

I’m working on a new video, but before that I wanted to add a small post as a way of an answer to a question I’ve been asked quite a few times already: where do all those buttons and toolbars that you’re using come from?  I know this is something that the more experienced user already knows, but it is a very real and very justified question when you’re just getting started. So here it goes.

Every time you open a document in SolidWorks, you are going to see a set of toolbars that appear there by default and that contain buttons for the most common features (commands) that you’ll ever need. You’ll notice that some of these toolbars and commands are available only for one kind of document and not for others.   For the most part, you’ll get by with these few commands, but every now and then you’ll need to reach out for something special or may need to use a particular set of tools. Here’s how to find them.

First, here’s how to add more toolbars. In the most general of all cases, simply go to Tools, Customize and click on Toolbars on the Customize dialog box that will open. Notice that, because the toolbars and commands are related to the kind of document you are working with, you will only be able to do this when a document (part, assembly or drawing) is open. Choose the toolbar you want to add from the list and it should show up like a small box, on the side of or even inside the graphics area. You can easily drag this box to wherever you want it to be. In SW 2007 (and maybe previous versions, I’m not sure) you can drag it out of the screen area and into the command manager with the rest of the toolbars.

In SW2008 and 2009, the command manager appears by default above the graphics area and the commands are contained inside tabs that replace the toolbars from previous versions. In SW2008, this command manager is docked above the graphics area. In SW2009, you can undock the command manager and position it somewhere else in the graphics area, but you’ll still find tabs, just the same.  You can add toolbars in the same way as described above for 2007, or you can add the commands contained in the toolbar in a tab in the command manager.  Just as before, go to Tools, Customize. The same dialog box will open, but this time you will also notice  a series of tabs in the command manager that were hidden before and that perhaps you didn’t even know you had. In the image below, those tabs are Surfaces, Sheet Metal, Weldments and Mold Tools, and are highlighted in a lighter shade of gray.  If you right click on these tabs and select Show Tab, you’ll be able to see them and select tools from them. 

Notice also the extra tab on the right side.  Click on it and a list of available toolbars will show up, choose from this list to include the toolbar of your choice in a new tab. In this image, I chose the Splines Tools and added the commands in that toolbar as a tab in the command manager.  

You can also click on Empty Tab to create a new custom tab and fill it up with any commands you may want to put in it, like all those commands that you use more frequently in your projects, etc.  By default, this empty tab will be named New Tab, but you can rename it by right clicking on it (while the Customize dialog box is still open) and choosing rename tab. Note: the custom tab won’t become visible until you actually add some buttons (commands) to it.

And how do you add the commands to the toolbar? Well, if the  Customize dialog box isn’t still open, go back to Tools, Customize  and choose the Commands  tab this time, browse the commands available  in the different categories until you find the one(s) that you need, then, click and drag the command to the toolbar or tab where you want  to add it. If you are creating a custom tab, for instance, you can have commands from many different categories all together in one tab. In this example, I created the custom tab My commands and added a couple of buttons to it. Notice that although they appear active while we’re dragging buttons to the tab, the Model View and Create Layout commands are really going to be grayed out because they’re not available for this kind of document.

So now you know where the buttons are coming from.

Learning how to properly do drawing and detailing in SolidWorks isn’t precisely the most exciting thing in the world, but it’s necessary, so I try to keep at it, even when it seems I’m making progress in an extremely slow fashion.

Anyway, I was learning how to create Annotation Favorites, when I noticed that something was different about Favorites for SW2007 and SW2008, when compared to SW2009. Well, first of all, an Annotation Favorite is any kind of annotation such as a note, weld symbol, surface finish symbol, geometric tolerance symbol, etc., that can be named and saved to be reused in the document.  They are called Favorites in SW2007 and SW2008, but renamed as Styles for SW2009. The extension of the file in which SolidWorks stores this information has also changed, but never fear, because you will still be able to use your favorites created in SW2008 and SW2007 in documents created in SolidWorks 2009. I’ll tell you all about it in a few minutes.

Using SW2008, I created a favorite by selecting a note (My Note in the image) and clicking on Add or Update a Favorite in the Note property manager on the left. I was prompted to enter a name for my Favorite, and so I named it My Little Note. 

The next step was to save this favorite as a file, so I could be able to reuse it in this or other document. Notice the extension .sldnotefvt given by SW2008. I saved this file in the annotations folder of SW2009 Design Library, just to see if I would be able to reuse it in a document created in SW2009.

And, yes, the Favorite was still available for use in SW2009.

Now, why did I do this? What made me wonder if I would be able to use the same favorites in SW2008 and 2009? Well, it’s just that, as I said before, the extension of the files for SW2009 is now different to the way it was for SW2008. In the following image, notice the extension .sldnotestl given to the same Note when it’s saved as a Style in SW2009, previously known as a Favorite for SW2008.

These favorites or styles can also be deleted and edited at any moment. To edit one of these favorites, simply make whatever changes you need to it, select it, click again on Add or Update a Favorite, select the name of the favorite you are updating from the list, and finally, save it again, same way you did before.

I know this little piece of information is extremely basic for those with lots more experience in SolidWorks, but believe me, I just found out about this one while working my way through the SolidWorks Drawings training manual. Well, you know there are multiple views you can choose from to display your part or assembly, right?  You have top, bottom, right, left, isometric, trimetric, etc.  Did you know you can also create and name your own custom views? I kind of suspected this was possible, because I had seen some parts used in other manuals that had views you don’t usually find available in the toolbar, like Reverse Isometric and such, but until now I had no idea how to do it. Well, it’s very simple, all you need to do is position your part and assembly just the way you want it or need it to be for your custom view by using Shift and the arrows, dragging it around with your mouse, using Roll, Rotate or whatever way works best for you, then click on View, Modify, Orientation to display a little menu of views (Note: you can also use Spacebar to get to the same menu).

From the menu, choose New View (second icon from left to right).

Type the name you wish to give to your new custom view.

And that’s it! Your new custom view will be available for you next time you need it and it will save you the work of dragging and rotating the part or assembly to achieve that particular orientation again.

The inspiration for this post came from a question a friend asked me about an alternative way to have a component in an assembly display in different colors, without using a configuration for each of the colors. He complained that the assembly was growing large in size due to all the different configurations. I suggested he used Display States, instead, since I remembered I had done something similar in the past, although I wasn’t exactly sure if it would produce a smaller file or not.  So, I decided to try it myself using an assembly I had just created in SolidWorks 2008. As it happens very often to me these days, while doing this I stumbled on something else that has changed since 2007.

As it turns out, Display States are no longer exclusive of a particular configuration. What does this mean? Well, in SW2007, every configuration had its own display states, that could be copied from one configuration to the other, but not exactly shared. In the past, whenever you created a new configuration, a new and unique Display State was assigned to it by default. In SolidWorks 2008, you can choose not to link the different Display States to any configuration in particular, which means they can be shared by all configurations in the assembly.  Why is this useful? Well, if you think about it, a Display State allows you to define different combinations of settings for the appearance of the components in your assembly: color, transparency, display mode, texture, whether  the component is hidden or showing, and RealView options, in case the RealView Graphics is on. This means that, for instance, you can define a Display State in which all similar components are hidden or transparent or a certain color or texture.  If you have configurations that use all the same components and these components only change in size or position, then you may very well benefit from creating Display States that apply to all configurations.  You create it once and it’s good for all!

So, how do you get started? Well, first of all, go to the Configuration Manager and there you will see the configurations on the top section and the display states on the bottom section. Right click on an empty area of the Display States section and select Add Display State from the menu.

You can add as many Displays States as you need this way. Notice the option at the very bottom of the Configuration Manager. It gives you the option of linking the Display State to the active configuration or leaving the Display States unlinked, thus accessible to all configurations in the assembly.  I created three Display States for my assembly. At this point I had only one configuration, so it made no difference whether I chose to link the Display States or not.

Next, you  can define the combination of settings for each of the Display States you just created by going back to the Feature Manager and showing the Display Pane (click on the >> that shows at the top right corner of the Feature Manager). Clicking on the icons that appear in the Display Pane for each component allows you modify that particular aspect of the appearance for that component in the assembly, for the active Display State. Here, for instance, I’m changing the transparency of one of the pistons.

You can also right click any of the icons in the Display Pane and a fly out menu will show up, giving you access to all the different settings for that particular component. From this menu, you can also add a new display state (Add Display State), rename the current display state, or change the current Display State, by clicking on Activate Display State and choosing a different one from the list.

If you have RealView Graphics on, clicking on RVAppearance allows you to change the PhotoWorks appearance, color and even transparency of your component.

As I said before, for my assembly, I created three Display States:  the first one with no changes at all, the second one where all the instances of Piston were colored blue, and the third one, where all the instances of Piston were made transparent.

At this point, I had only one configuration for the assembly, so I decided to create another two configurations, just to see how the option to link or not link worked like. Notice how, when the Display States are not linked, all the configurations (even those that aren’t active) have the same Display State: the one that is active at the moment. In this case, Display State 2 is active.

Display States can also be driven by a design table, if needed.

As a side note, and to answer my friend’s original question, I did try to do the same by using three configurations, instead of three Display States. One configuration with no changes, one with all the instances of Piston colored blue, and one with all the instances of Piston set to transparent.  The resultant file is a little bigger in size than the one that would result from using only one configuration with three Display States. The difference, however, is only of 200 MB or so. I remember reading somewhere in Matt’s SolidWorks Bible that using Display States instead of configurations in order to control the display of parts can actually improve the performance of the assembly, since changing configurations requires reading the model geometry again, plus, as I confirmed, they also take up additional file space and CPU time.

I’m still in the adjustment phase with SolidWorks 2008. I’ve been trying hard to resist the urge to do everything in SolidWorks 2007, just because it’s the “familiar” environment and I already know where everything is. Instead, I’m trying to spend more time working on SolidWorks 2008, and, as a result, I keep finding new things (or things that have changed) here and there.

This time, while practicing my top-down assembly modeling skills, I ran into something called “Virtual Component”.  Huh? Is it virtual because it doesn’t really exist? Well, not exactly. Apparently, in SolidWorks 2008, when you create a component in the context of an assembly (top-down modeling), you are no longer required to give it a name and save it right away, like before. Instead, the in-context component is saved inside the assembly document. You can work on it, delete it, insert more instances of it, pattern it, etc. You can do anything you would normally do with an in-context component! Anything? Yes, you can even create a component with no external references. “Hmmm, but what’s the catch?” you may wonder. Everything has a catch! Well, I haven’t found one yet. So far, the only catch is that, at some point, you may want to save those components as individual files… and you can do that too, so I guess it’s not much of a catch. The beauty of this is that, in the end, you only keep those in-context components that you really want, and the rest of them, the ones that used to accumulate inside your folder while you were changing your mind, those aren’t even there.

I tried this new functionality with a small assembly.  A simple experiment first, just to understand how it worked. So, I created an assembly, using this little part that came with the “What’s New?” document, as part of a tutorial for the configurations property manager.  The part (My_two_bolt_flange) has different configurations, and I wanted to see what happened to the in-context part when switching configurations for the referenced part and/or making changes to it.

I began by doing exactly the same I would’ve done in SolidWorks 2007 in order to create an in-context part: click on Insert Components, New Part, and choose a plane or a face where to place the in-context component’s base sketch. This will become the Front plane for the in-context component. In my case, I chose a face on one of the boss features of my first component, My_two_bolt_flange. Notice how a new part is added to the feature manager (Part7^My assembly), but I’m never prompted to name it or save it at this point.

I create my first sketch in this new part by converting the circular edge of one of the cut features in My_two_bolt_flange. Part7^My assembly is now an in-context part, referencing to geometry from My_two_bolt_flange.

Finally, I extrude the sketch and finish creating the part. I exit the Edit Component mode and go back to editing the assembly. This is exactly how I would’ve done it in SolidWorks 2007, except that here I didn’t have to save the part or even name it.

At this point, if I change the configuration of the referenced part (My_two_bolt_flange), the new in-context part updates too.

The same happens when I make changes to the referenced part. Here, for instance, I changed the diameter of the cut feature in the default configuration from 0.5 in to 0.7. After rebuilding the assembly, the new part updated, as well.

When the time comes to save my work, I am finally asked if I want to save the part I just created internally or if I want to save it as an individual file. If I choose to save inside the assembly, no other files are created. Next time I open my assembly, if any changes have been done to the referenced part (My_two_bolts_flange), all the parts in the assembly will update too, same as always.

If I want to save the part as an individual file, all I have to do is right click on it in the Feature Manager, select Save Part (in external file) and a dialog box will allow me to rename the file and select a path for it, which can be the same as the one for my assembly or a completely different one of my choice.

I like this new functionality, but I do wonder if it has the potential of creating huge assembly files.  As far as I know, assembly files used to be small in size, because they didn’t actually contain any of the parts. These new assembly files that result from using virtual components do contain some of the parts inside of them. This has to make them bigger. But how much of an issue can this really be? I compared the size of an assembly with the part included as a virtual component and the same assembly with the part saved as an individual file. The size of the one with the virtual component was 388 KB, versus 184 KB for the one that had none. That seems like a big change, but then again, it may not mean much for the overall performance if the assembly continues to load as fast as before. I didn’t notice any changes between the two assemblies, but that may also be because they are very simple, with only two components. What are your thoughts on this new functionality? Do you use it? Do you notice any change in performance?