Once upon a time, a blogger asked a question!

The members of the blog squad do communicate to each other on a variety of things we are interested in, or may be working on.  We “support” each other in our efforts to help keep learning more, and improving our own experiences.  Every once in a while we come across something that needs to be shared with others.

In short, here was the question:

In the industry that I am in I do not get the chance to get in a lot of different/deeper areas of SolidWorks.  I rarely get the opportunity to use the surfacing and weldments features in SolidWorks, but I want to.  I want to be able to help other users if they run into problems in these areas.  Now I can only do the tutorials so many times before that gets extremely old.  Here is where you come in, do any of you have ideas of how I can continue to use these features in my spare time without using the tutorials?  Any ideas or suggestions would be greatly appreciated.

Here was my initial response:

You are in a similar situation I am in.  At my work, because of our products, we are limited in the features we need to use to model our products (blocky stuff).   You are on the right road, by going out and exploring other SolidWorks features.  The tutorials are great, but they tell you how to use SolidWorks features to create a specific model.  If you want to do more of these, check with your local user group an see if someone has advanced training manuals you can borrow, and go thru those exercises. 

I believe the best thing you can do is to look at other products, and then try to model those products in SolidWorks.  I believe this experience is more beneficial because it provides you the opportunity to develop a thought process to effectively and efficiently model various products using a variety of SolidWorks features.  Once you have modeled something up, don't stop there.  Model it up again trying different features and see if it's easier or harder.  By doing this, you are learning from your own experiences, and you can keep building on those experiences.

I have been doing this for several years and the experience has benefited me in my work because I now have a tendency of looking further "outside the box" while modeling something more complex.  Every once in a while, we come across something we have not done before, and I'm the one who gets to experiment with the various methods of creating the model(s).  It makes work more a little more fun when you can do this.

There were a few bloggers that also tossed in the following ideas/comments: Some of these ideas have been summarized.

• The best thing to do is walk around the house and find things that look interesting to model.  Remote controls, silver ware, kids toys, kitchen items are all things that come to mind.  Even something as simple as a spoon or fork can be a challenge. Random household items would take you a long way. Just think of the multitude of random shapes throughout the house. Vases, figurines, toilets, toys, statues, the list is endless.
• For me I use a hobby to fill the void. I build bikes (pedal powered) and that is a great way to get into weldments. Also I made my deck using weldment features, it worked really good. I also explore what the functions do in each area and ignore the name you may find (actually will find) new and cool uses for a function. You see, for example, in mold tools there is a cavity function that is great if you make weldment assemblies and it will cut a tube in one move verses 3. Just because you don't do weldments, or things like does not mean you can’t use the features in the weldment or mold tool toolbars.
• I guess all we can do at some point is try to come up with ways to model things around us.  I started doing that with my son’s Legos and other toys and things around the house. Many times they are not as easy as they look!  I also keep an eye for when someone posts files about what they’re doing in the forums.  Maybe you could come up with your own workbook! My godfather used to say to me that when you want to learn more about something, the best way to do it is to try to teach others about it.
• Matt’s Surfacing Book will absolutely help you get a better understanding on the power of using surfaces to create products.  This is one of the areas I’ve been learning about in my spare time for some years now.  Most of the knowledge I have gained in doing this on my own time has resulted in me being able to go after projects here at work that we couldn’t otherwise do in the past.  The result is that I am now continuously getting challenging but “fun” projects and my employer truly recognizes and appreciates my efforts.
• There's not always enough time to grab something new and model away. You're familiar with the stuff you do at work, plus you have interest in the other functionality which is key. If you know a little about, wrapping, combining, curving, projecting, radiating, weldment-ing?? cavity-ing??? you'll get yourself in enough trouble, to figure it out dang quick and redo it even better... or try another way.
• Get the SolidProfessor on-line courses for some funky stuff. That might give you some ideas.  I agree in general with people who say model stuff at home. That's cool. But there are two traps with that: getting too detailed, and not getting detailed enough.  Spoons are easy if you fake them, but difficult if you try to do them correctly. Try to model a pair of Oakley sunglasses. I dare you.  And then there's the question, do you just want to do a large project, or a complex project?  With complex data, use some sort of starting point like a digital photo or point cloud or scanned hand drawings, or whatever.
• You could also pick up a copy of a drafting class book.  They are usually loaded with dimensioned ISO views, and also have problems in them to work out.  It's how I taught myself 3D modeling in Autodesk Inventor (before I saw the light!) when we moved from AutoCAD.  I think that this is a great way to learn new ways of using the software and will expose you to all different kinds of components and modeling practices.
• How about the books by David and Marie Planchard? They may not be big on the narrative style, but they are LOADED with samples and exercises, and there’s so many of them!  I’ve begun collecting them…   The kind of stuff you don’t find in bookstores, like training manuals, videos, etc. Also look among used books. Sometimes you can find treasure.
• Back in 98-99 before there were community college classes, my only resource were the Planchard and Planchard books.  I taught myself from those books, and the rest all came from pure use of the software from day to day.  I would bet that a large portion of us have modeled that flashlight they used in their books over the years.

And the thanks from the first blogger:

You are all amazing!  Thanks to ALL of you for helping me with this.  I really appreciate the time that you took to respond to me with your thought about this, it’s unbelievable!  Modeling the daily stuff around me is something I never thought of.  I guess that goes to show that the obvious stuff is not always so obvious.  Thanks again and I hope that we can all get together again hopefully sooner than later.

In Summary, Explore and Experiment!

To be more effective with SolidWorks, or any other software you are using, you need to explore functionality you normally don't use.  Find something you normally would not model, and model it up to get more familiar with other capabilities of the software.

Good Luck!

Model Rebuild Performance

In the past, I have seen some discussions on whether it’s best to add radii to sketches, or use a fillet feature to obtain round corners on flat parts.  I have always been a proponent of creating the part the same way it would be manufactured, where each feature in the Feature Manager Tree would represent a separate step in the fabrication of the part.  I am also a proponent of adding cosmetic (non-functional) features separate from the features that are important to the model.  These cosmetic (non-functional) features should be added near the end of the Feature Manager Tree so they can be suppressed to simplify the part.

I was recently working on trying to improve the rebuild performance of a model of a part that is used on a product I helped develop.  SolidWorks would pause every time an assembly was loaded that contained this part.  We were not talking about a one-time use “special” model.  This particular part is an integral component of several current and future products.  This meant that the model was subjected to being loading (within parent assemblies) several times during the product development.  This part has cutouts are used in several parent assemblies, therefore these cutouts could not be suppressed to simplify this part.  That started an investigation into how I could improve the load and rebuild times for this model.

The model is a formed angle that contains cutouts that spanned across the bend line and had filleted corners (for the cutouts).  The cutouts were also patterned.  After checking the Feature Statistics, I found that the patterned cutouts took the longest to rebuild.  This led me to do some experimenting.  The results listed below are not from the part, but they do represent some of the techniques that can be used to create these features in the model.

Scenario 1:  Cutouts created between “Flatten Bends1” and “Process Bends1” features
How the model was created: Create sketch of formed part, and use “Extrude-Thin” to create the part.  Convert the model to a sheetmetal part via “Insert Bends”.  Roll-Back before “Process-Bends1.  Add square-corner cutout.  Add feature fillets to the cutout.  Pattern the cutout and fillets.  Move the Roll-Back bar to the bottom.  Assembly Statistics reveals that the Process-Bends1 feature takes about 59.0 to 66.5% of the rebuild time.  Rebuild times: .34 sec w/ fillets, .30 sec w/o fillets.  When the corner radii were added to the sketch, the rebuild time increased to .36 sec.

Scenario 2:  Cutouts created between “Unfold1” and “Fold1” bend features
How the model was created: Create sketch of formed part, and use “Extrude-Thin” to create the part.  Convert the model to a sheetmetal part via “Insert Bends”.  Create Unfold1 feature.  Add square-corner cutout.  Add feature fillets to the cutout.  Pattern the cutout and fillets.  Create Fold1 feature.  Assembly Statistics reveals that the “Flatten-Bends1” feature takes about 41.9% to 47.3% of the rebuild time.  Rebuild times: .38 sec w/ fillets, .33 sec w/o fillets.  When the corner radii were added to the sketch, the rebuild time increased to .38 sec.

Scenario 3:  Cutouts created and patterned before “SheetMetal” feature
How the model was created: Create sketch of formed part, and use “Extrude-Thin” to create the part.  Convert the model to a sheetmetal part via “Insert Bends”.  Create Unfold1 feature.  Add square-corner cutout.  Add feature fillets to the cutout.  Pattern the cutout and fillets.  Create Fold1 feature.  Assembly Statistics reveals that the “Flatten-Bends1” feature takes about 47.3% to 48.5% of the rebuild time.  Rebuild times: .59 sec w/ fillets, .52 sec w/o fillets.  The way that this model was built, the appropriate radii could not be added to the sketch.

Scenario 4:  No use of “SheetMetal” feature.
How the model was created: Create sketch of formed part, with bend radii added to shetch, and use “Extrude-Thin” to create the part.  Add square-corner cutout.  Add feature fillets to the cutout.  Pattern the cutout and fillets.  Rebuild times: .04 sec w/ fillets, .09 sec w/o fillets.  When the SheetMetal feature was added at the end of the feature tree, the rebuild times increased to: 56 sec w/ fillets, .48 sec w/o fillets.  The way that this model was built, the appropriate radii could not be added to the sketch.

In this case, the use of the fillet feature was more beneficial over adding radii in the sketch, because the fillet could be suppressed to reduce the rebuild times by a few tenth’s of a second.  This may seem insignificant, but in the more complex part I was building, this provided a consistent reduction of 40% (5 seconds) off of the rebuild time.

Something else to note here is the use of the Sheet-Metal feature.  Even though this feature did significantly increase the rebuild times, it is still necessary to obtain a Flat-Pattern of the model.  For a simple model, if you can build your features into the model before adding the Sheet-Metal feature, you can then suppress the Sheet-Metal feature at the end of the feature tree to reduce rebuild time.

Your models and “mileage” will vary.  These are only a few simple guidelines to consider when building model.

• Model features can be suppressed, sketch entities cannot.
• For every model you create, build the relevant (or functional) features first, then add the cosmetic (non-functional) features later in the tree.  This allows you to create simplified versions of your model by suppressing the cosmetic (non-functional) features.
• Keep in mind that how, when and where a feature is built in the Feature Manager Tree may affect the rebuild times for that feature and the remainder of the features in the model.
• Due to the calculations behind generating non-planar (flat) surfaces (radii, revolves, loft, sweep, dome, etc…) have an adverse affect on rebuild times, you should limit your use of them, or put them later in the feature tree so they can be suppressed to reduce rebuild times.
• Using simple sketches makes it easier for you and other users to determine what is being created.
• Use of fully defines sketches reduces the “guesswork” for the features SolidWorks is expected to generate.

Good luck.

Helping assembly mates survive promotions and demotions

Many times it may be necessary to move components (parts or assemblies) up or down a level or two within the assembly tree.  This is sometimes referred to as promoting or demoting.  When this is done, SolidWorks will move many of the mates with the components.  When promoting or demoting components, you may experience unforeseen mate errors.  Here are a few things to look for, in a methodical order, before you get too excited and think that SolidWorks has corrupted your assemblies.

• Component(s) that are “Fixed” in space that should be “Floating”.  SolidWorks maintains the fixed/floating status of component(s) as they are moved between assembly levels.  If a component was “Fixed” when you started the move, it will still be “Fixed” when it is moved to another assembly level.
• Sub-assemblies(s) that were “Flexible” but are now “Rigid” after moving them to another assembly level.  SolidWorks defaults assemblies to a “Rigid” status after they have been moved between assembly levels, similar to inserting a new assembly.
• Referenced configuration of component may not be set as intended.  In some cases, I have seen SolidWorks set the referenced configuration to “Last used configuration”.
• Check and verify mate dimension direction for distance and angle mates.  Check and verify mate alignments for angle mates.
• Multiple mating schemes (ex: open, closed, etc…) that position/reposition the component(s) within the assembly.  Some of these mates may need to be suppressed in one assembly configuration, and unsuppressed in another configuration.

Fixing mate errors due to multiple mating schemes will probably take the longest to weed thru.  SolidWorks provides many tools for resolving mate errors due to multiple mating schemes.  Use SolidWorks’ Mate Diagnostics Tool to evaluate and reduce these errors.

You should pay special attention to advanced mates to ensure that they are properly related to the correct components.  When the “Width” and “Symmetry” mates were first, there were issues where mates disconnected from the surfaces when one component was promoted/demoted, and the other component was not.

Cavities can be good for you!

A coworker approached me about a project he wanted to do at home, which was to make a dovetail jig for the many drawers he was going to make.  What he needed help on was making the dovetails slots and pins, within SolidWorks, and maintain associativity.

The first thing I thought of was to use SolidWorks’ Cavity feature.  The Cavity feature is commonly used for creating cavities in molds for parts that are to be molded.  For those who don’t create molds, this feature becomes a rarely used, and sometimes forgotten capability.

Here is a quick review on how to use the Cavity feature for the dovetail example.  I have also provided simple models so you can try this yourself.

• Start with 2 parts.  TAILS.sldprt has the dovetail pins that are sized and shaped to match the profile of the router bit being used.  SLOTS.sldprt does not have any profile for the dovetail slots, but has additional material to create an interference at the dovetail joint. (Included in zip file)
• The assembly JOINT.sldasm, includes the TAILS and SLOTS parts which are mated to ensure an interference exists at the dovetail joint.  (Included in zip file)
• Open the assembly and select the SLOTS (Salmon) component, and activate “Edit Component”.  In the pull-down menus, go to “Insert, Feature, Cavity.”  Under Design Components, select the TAILS (Yellow) component and make sure the scale is set to 0.00%. Click the check mark or OK to complete.  You will see that the SLOTS.sldprt (Salmon) part now has a new feature.
• On the Assembly toolbar, click on “Edit Component” to complete the edit.
• Open the SLOTS.sldprt model and you will see the dovetail slots have been created.

Here’s what happened.  SolidWorks’ Cavity feature removed the interference between the TAILS and SLOTS components by removing the “interference” material from the component that was being edited in the assembly, in this case, the SLOTS component.  When this is done, an in-context reference is created In the SLOTS model that referenced the JOINT assembly and the TAILS model.

Keep in mind:

• Whenever the TAILS model is revised, you my need to open and rebuild the JOINT assembly for the SLOTS model to be updated.
• Changing the positional relationship between the TAILS and SLOTS components within the JOINT assembly will cause the SLOTS model to update.
• When using in-context references, do not delete any of the referenced (in this case the JOINT.sldasm and TAILS.sldprt models) models, or the references in the SLOTS.sldprt model will break. 

Can you think of any other examples where you can use the Cavity feature?

Blockhead does Surfacing

Ok, I admit that the title for this article is a spin off of the title "Surfacing for Blockheads presentation by Ed Eaton", but hey it's true, I am a blockhead and I can do some surfacing.  The intent of this article is to identify a few examples where a user may need to incorporate simple surfacing techniques in their "blocky" type models.

One recent project I worked on was a "tub style" part, where a Y-shaped center section was raised and shaped like a dome, and the outer ends of the Y-shape curving back down to below the rim.  This part was to be thermo-formed, so I also had to have uniform thickness, I had to incorporate draft and also round the edges, much like doing a casting.

I started with an extruded feature for the tub to identify overall (center) height, diameter, and rim height.  The next step was to determine an efficient way create the domed Y-shape rising up from the center.  If I use SolidWorks' Dome feature, or create a cut revolve at the top, I would have to create my cuts using the offset from surface, then link those offsets to all dimensions relating to the thickness of the tub.  Another was to do revolved cuts from the side, but that was hard to keep a uniformed dome in the center.  To keep the part simple for me, and others, to work on, I quickly determined that these were not the best ways to go. 

I knew the best way to maintain a uniform thickness on this type of part was to use SolidWorks' Shell feature.  In the end, I created an arc, with one end perpendicular to the centerline, and the other end extending beyond the outer side of the tub, I then created a revolved surface with this arc.  This gave me a surface that looked like an upside down saucer, or a dome shape.  The top of this arc represented the highest point of the underside of the tub, so I had to allow for the part thickness here. This gave me a simple domed surface that I can cut to.  Using a surface in this manner provides a consistent face that does not change when using solid modeling cuts and extrudes.  If the radius or heights (center and outer edge) of the dome feature are changed, all features referencing the domed surface are automatically updated.

All future cuts in this model were created starting at the bottom of the tub, drafted, and cut up to the domed surface.  Once all of the cuts were completed, I could fillet the edges, and shell out the part to the required thickness.

This model in the BlockheadTub edrawing has been made semi-transparent so you can see the domed surface (salmon color), in relation to the part that was created.  You would typically hide the surface so it is not seen where this part is used.  I know that this is not the perfect surfacing scenario.  I know that I could have used face blend fillets.  I know.... HEY! This is just an example, and I am not an Industrial Engineer, so give me a break!

I recommend for everyone to take some time to look at, and step thru the SolidWorks' Online Tutorials and some Training Manuals, and try out some of the features in SolidWorks that you normally don't use.  Even if you feel you may never use these features in the future, the experience may become useful when you least expect it.

Changing Habits

The computer keyboard is based on the typewriter, which was designed for use with two hands.  With text based applications, the keyboard may have been the only way to enter data and move around in the application. 

The computer mouse, which was designed for use with one hand, helped reduce some typing on the keyboard by providing the capability of pointing and clicking to get things done.  The mouse is a huge benefit for getting around in graphical based operating systems (Windows), applications (Office) and CAD (SolidWorks). The mouse keeps one hand busy, but what about the other hand?

Besides using the mouse, there is another way to get around in an operating system and applications, and that is by using the keyboard and keyboard shortcuts.  Listed below are commonly used shorts, and a few that you may not even be using.

Keyboard Shortcuts in Windows

• "CTRL-X", "CTRL-C", "CTRL-V" are commonly used for cutting, copying and pasting data, but did you know that "SHIFT-DELETE", and "SHIFT INSERT" can also be used for cutting and pasting?
• "CTRL-Z" provides a quick undo of the last command.
• "CTRL-N" can be used to create new files, while "CTRL-O" and "CTRL-S" are used to access the open and close dialog boxes.
• "CTRL-P" will bring up an application's printing dialog box.
• "ALT-TAB" brings up a window to switch between applications, but did you know that "CTRL-TAB" will switch between open documents within an application?
• "ALT-ESC" works like "ALT-TAB", but immediately displays the application.  It cycles thru the applications in the order they were opened.
• "ALT-F4" closes an application, while "CTRL-F4" closes the current document while keeping the application open.
• "F10" activates the program's menu bar, which allows parsing thru the menu with the arrow keys.
• There are many more keyboard shortcuts available in Windows that are now listed here.  To find our more, look for "Windows keyboard shortcuts overview" in the Windows Help and Support Center.  You can access this by pressing "F1" while looking at your computer's desktop.

Keyboard Shortcuts in SolidWorks

• Nearly everyone who uses SolidWorks knows that the "Z" and "SHIFT-Z" are used to zoom and zoom out while viewing a document, and "F" will fit the document to the screen.
• And most people know that using the arrow keys will rotate the model a predefined increment, but did you know that using the "SHIFT" key in conjunction with the arrow keys will rotate the model by 90°, and using the "ALT" key in conjunction with the arrow keys will turn the model clockwise or counterclockwise on the screen?
• Pressing the "SPACEBAR" will bring up the View Orientation" menu, but did you know that combining the "CTRL" key with a number key will rotate the model to a specific view?  Example "CTRL-1" will rotate the mode to the Front view, and "CTRL-5" will rotate the mode to the Top view while "CTRL-7" will rotate the mode to the Isometric view.
• Nearly everyone knows that "CTRL-Q" will rebuild the model, and it's features, but did you know that "CTRL-B" just rebuilds the model, and "CTRL-R" redraws the graphics screen.
• There are many more keyboard shortcuts available in Solidworks that are now shown here.  To find our more, look for "Keyboard Shortcuts" in the SolidWorks Help File.
• SolidWorks also allows you to define your own keyboard shortcuts.  Just go to "Tools, Customize", then go to the "Keyboard" tab.  Find the command, then define the keyboard shortcut you want to use.  For more help on this, look for "Customize Keyboard" in the SolidWorks Help File.

So you still want to use the mouse!  Here are a few things that you should be aware of.

Using the middle mouse button in SolidWorks

• Pressing the Middle Mouse button while dragging the mouse will rotate the model.  Holding the "CTRL" while doing this will PAN the model on the screen, and holding the "SHIFT" while doing this will ZOOM the model on the screen.
• Within a drawing, pressing the Middle Mouse button while dragging the mouse will pan the drawing.  Holding the "SHIFT" while doing this will ZOOM the drawing on the screen.
• Scrolling the wheel on a wheel mouse will also ZOOM the model in relation to where the pointer is on the screen.
• For more help on this, look for "Middle Mouse Button Functions" in the SolidWorks Help File.

Additional input devices:

• The trackball is a nice replacement for the mouse because you don't have to keep moving it around on the desk, just spin the ball to move the cursor.  You can even lean back and set the trackball on your lap, and still mouse around the screen effectively.  There is also a finger version of the trackball that you may want to evaluate to see if it meets your needs.  It's smaller, lighter, and fits on your finger.
• 3DConnexion has a line of input devices that can keep your other hand busy while in SolidWorks.  You can get something as simple at the SpaceNavigator, which provides the capability of rotating, spinning, panning, and zooming documents within SolidWorks.  There are also 2 buttons on this device that you can reprogram as you prefer. You can step up to the SpacePilot or the SpaceExplorer, both of which give you more buttons that you can program to meet your needs.  By moving these functions to another device, and hand, you can reduce some of the movements you are currently doing with just the one hand.

NOTE: This article was written in response to a message I found on the comp.cad.solidworks newsgroup concerning a problem a computer user was experiencing that may be related to Carpal Tunnel.  Some of these ideas came from a co-worker who has unrelated problems with his wrists, and he is always looking for different means of minimizing his input at the computer. 

Please keep in mind that your needs, and the available equipment, will most likely dictate your working habits.  The intent of this article is to highlight possible alternatives to constantly using a one handed mouse for getting around in the operating systems, office applications, and CAD programs.