If you are one of the early adopters of Windows 7 you have probably already fell in love with the new taskbar design.  It gives you a built in dock type feature so that you can quickly access and launch your favorite programs.

Well, Darin Grosser, a former AE Model Mania winner, has posted about how to add SolidWorks to the new Windows 7 taskbar AND have it act like the rest of the programs you can add.  The problem that he was seeing and that I have seen is that you could add the button to the taskbar but when you clicked it to launch SolidWorks it would open another instance of it instead of launching that icon.  To see the correct way to add SolidWorks to the taskbar read his blog post.  Follow the link below.

SolidWorks Icon on the Windows 7 Taskbar – DASI Solutions Blog

Anna Wood did a blog post about her frustration with SolidWorks 2009 SP 5.0 Not Allowed To Install On Windows 7 w/ SWIM.  She later updated her post with how to get it to install using manual downloads from the Customer Portal.

This morning in my attempt to also upgrade to SolidWorks 2009 SP 5.0 on my Windows 7 machine I stumbled across another workaround for this problem.

Windows 7 (and Vista) include a compatibility tool that allows you to run programs for other versions of Windows.  The workaround that I came across this morning includes telling the SolidWorks Installation Manager to run in compatibility mode for Windows Vista.  To activate this option you need to go to Start > All Programs > SolidWorks Installation Manager > Check For Updates.

Once you are to this point RMB click on Check For Updates and select Properties.  This will open up another window like the image below.  Click on the Compatibility tab and in the Compatibilty mode box check the box by Run this program in compatibility mode for and then select Windows Vista (Service Pack 2) from the drop down list.  I imagine that the other option for Windows XP and Windows Vista would work as well for this but I used the Windows Vista (Service Pack 2) setting.

Once you are finished, click Apply and you are all set to go to download the SolidWorks 2009 SP 5.0 upgrade.

So how many of you have ever seen the dreaded “Failed to save document” message like the one on the left?  Usually this warning appears after you have spent ALL day working on an uber complicated assembly and there you sit, right?

Well, I think I have found a way to not lose all of the work you put into that assembly since your last save.  Here are the steps to save yourself from the wrath of you boss when you have to explain to him that the last how many hours have been lost on that hot project you are working on.

1. Do a “Save As” of the assembly with a different name inside the same folder as the original assembly.
2. Close all SolidWorks files, saving what you can.
3. Delete the original assembly (take note of the EXACT file name).
4. Using Windows Rename, rename the new assembly to the file name of the original assembly.
5. Open assembly and you should be where you left off.

This method especially works well when you have in-context relations in that assembly.  By renaming the newly created assembly to the name of the original you will regain all of your in-context relations.

I hope this works for you as well as it worked for me.

Image courtesy of SolidSmack.

Today I sat in a webinar hosted by my VAR (DASI Solutions) called “A Healthy SolidWorks is a Happy SolidWorks”.  The webinar talked about a variety of things in regards to making SolidWorks run as smooth as can be.

One thing that I learned from them was this overlooked paragraph on the Hardware and Graphics page in the SolidWorks Customer Portal.  If you purchased your Graphics Card from the computer manufacturer with your computer, you are going to want to select your computer manufacturer in the Vendor section and not the Graphics Card manufacturer.

To check out other cool tips & tricks head over to their new blog and see what they have to say!

Thanks Jerald!

The title kind of sounds like it could be the headline of a relationship article but this post is actually going to be about fully constraining your model in an assembly.  When inserting parts inside of an assembly it is really easy to fix the part and continue on.  This allows you to fully constrain a part so that it doesn’t move and it is extremely quick and easy.  However, as easy as it is I am a major opponent to the practice of mating because it is easy to quickly float that part, move it a very little amount and fix it again and no one would ever know.  That is until the part gets made and stuff comes out wrong.

As is with most things in SolidWorks there is an alternative way to quickly fully constrain a part with only a few quick clicks.  When you insert a part into an assembly you can mate the origins of the part with a coincident mate and select “Align axes”.  How you may ask, where here you go.

To start simply insert a part into an assembly.  Select the origin of the part you just inserted and the origin that you would like it mated to.  In the picture below you will see that I want to mate the origin of the part I inserted to the origin of the assembly.  After you select the 2 origins select the mate command to begin the process.

Automatically when you do this SolidWorks will select the Coincident mate as your choice, which is correct.  Here is where you will notice one difference from what you would normally see with the coincident mate.  Underneath this mate you will see a check box for the ability to Align axes.  This is automatically selected for you.  If you would wish to be able to rotate around the axis you would want to uncheck this option but for what we are trying to accomplish you will want to leave it checked.

Now all you have left to do is accept the mate and your part is now fully constrained inside the assembly as shown below.

Now this option might not always work for you but with a little thought into what you are hoping to accomplish in your assembly when making the part you may be able to incorporate a little design intent so that you are able to use it.

Well, there you have it.  Another alternative to a SolidWorks process that is a little safer than just fixing the part wherever it may land in the assembly.  I personally still like to mate all 3 planes of my part file to something in the assembly but that is just a personal preference.  How do you fully constrain the parts in your assemblies?  Let me know!

Just like what triggered my post last weekend “rocksolid tutorial: modeling a variable profile helix cut” I was recently asked a question by a member of my user group about how to simulate the stroke of a cylinder in SolidWorks.  So here we go, this is how I would simulate a simple cylinder stroke in SolidWorks.

As you can see in the above picture I have quickly assembled a bottom plate (green) that is housing a gas cylinder (yellow) in a pocket.  I also have a top plate (red) that is mated to the bottom plate with a distance mate called “open/close distance” which we will discuss later.  My gas spring was modeled with a simple single sketch profile revolve as you can see below.

By creating my gas spring as a revolve it is extremely easy for me to add a coincident mate between the top of the edge (which represents the end of the gas spring cylinder) and the bottom edge of the top plate.  You can see that I have both of those entities highlighted in red in the above picture.

Once you I added this relation you can see that the sketch of my gas spring is now fully defined.  You will notice that I also have added a driven dimension on the overall length of the gas spring which I can monitor to make sure that it does not exceed the limits of the stock spring.

Once I have done that you can exit your sketch and stop editing the part in your assembly.  Now you are ready to edit the mate that I mentioned earlier.  I have named this mate “open/close distance” so that I can quickly find which one I need to change.  By editing this mate you can simulate the top plate moving downward towards the bottom plate therefore compressing the gas spring cylinder.  You can see in the above picture that my distance “open” distance is 5.170in.  When I change this value to 4.170in., which is my closed distance (shown below) you can see that my cylinder compressed like I am wanting to see.

This is just a quick and easy way to simulate this cylinder compression.  As is with most things in SolidWorks, there are many ways to accomplish this exact thing.  If you prefer using an extruded boss/base cylinder you can use the “Up to Surface” option which will result in the same results.  If you have another favorite way to do this type of thing please feel free to share.

This week I was sent an email from a member of my user group with a modeling challenge.  They needed to model a helix cut that had different widths at the start point and end point.  I first thought that this could get pretty involved with different sketches and profiles but after playing with it for a few minutes I realized that it is actually quite simple to accomplish this.  Here are the steps I took to get this variable profile helix cut.

I started the model by creating a simple shaft with a chamfer on the top.  I then offset a new plane off of the top plane that I want to use as the beginning (or ending depending on which way you think) of the helix cut.  You can see these first couple steps in the above screenshot.

Next I created the 2 sketches that I want to use for my beginning profile (shown in red above) and my ending profile (shown in yellow above).

Then I created the helix that I want to follow by starting it on my helix start plane and telling it to do 1 revolution in the distance to the bottom of the shaft.  The helix I created is shown in blue in the above screen shot.

The next step is where I actually create the cut.  I used the “Lofted Cut” command.  For my 2 profiles I used the 2 sketches that I created earlier.  Now 1 thing to keep in mind when doing this is that we you select the sketches SolidWorks puts a green point at the closest end point of the sketch.  You will want to make sure that those end points are at the corresponding points on both sketches.  You can simply drag and drop the points to to the correct location if SolidWorks misinterprets where to put them.  Next, I used the helix that I created as the Centerline Parameters of my loft.  This allowed my loft to rotate around the part like I wanted.

Voila, it worked and I achieved the desired variable profile helix cut that I wanted.  If you have another way to accomplish this same profile please feel free to share.

A couple of years back one of the enhancements to SolidWorks was the thumb wheel that appears underneath the dimension in the modify box that appears as shown above.  If you are not familiar with this feature and just thought it was a cute and cuddly graphic that they added you need to know what this does first and foremost.  By simply clicking on the thumb wheel you can drag it either left or right to increase of decrease your dimension, pretty nifty huh?

Changing Your Increments

Now depending on what you use SolidWorks for you may want change the increments that the wheel changes your dimension.  Piece of cake!  All you need to do is go to Tools > Options > System Options > Spin Box Increments.  Here is where you get some different options.  There is 2 different length increments that you can preset, English units and Metric Units.  Then you have the ability to change Angle increments as well.  If you are working on more precise designs you may want to set these increments smaller but if you are working with wide open tolerances you may want these larger.  Totally up to you as long as your mom, dad, wife/husband, kids and the creepy neighbor down the street approve or your decision.

Changing on the Fly

You thought we were done already didn’t ya?  Not so fast!  There are always those times when you want to tighten or loosen up what you set your thumb wheel increments to.  Instead of having to go in each time and change these you can sort of kind of do this on the fly.  By holding down the Ctrl key while spinning the thumb wheel it will increase your set increments times 10.  So lets say you have your increments at 0.10in (as shown above), by holding down the Ctrl key your increments will now be 1.0in until you stop spinning and release the key.  Likewise, if you hold the Alt key while spinning it will decrease your set increments divided by 10.  So in the previous example your increments would be 0.01in.  Nice and simple!

Source of the Information

This is a tip & trick that I learned from Mark Biasotti at the West Michigan SolidWorks User Group meeting that was held on Tuesday, May 12.  This is the awesome kind of stuff that you learn at user group meetings and the best thing about it is that his presentation was on surfacing, but even if that topic is not your forte you can still pick up great tips and tricks like this one.  So if you are not an active or regular member of a user group in your area you need to become one.  If there is not a group in your area, let me know and I will get you the contact information of someone that can hopefully help you start one.

I have been accused in the past of being sort of any organizational freak.  I am one of those people that usually does not like stacks of papers on my desk and have more labeled hanging file folders than you can shake a dead squirrel at.  This is why I have become a huge fan of using folders in the FeatureTree to organize.  Folders can be quickly added inside your part and assembly files by RMB clicking multiple features, parts, or subassemblies and selecting “Add to New Folder”.  Why would you want to do this you might be asking?  Well, that is a perfectly legitimate question that I am hoping to answer for you in this post.

Why?

As I stated above the answer is simple, organize and clean.  When you are working on the 500+ feature part or that 750+ part assembly wouldn’t you want to keep your FeatureTree as short as possible so you can easily find features or parts as you go.  I am never a big fan of scrolling, then scrolling some more, then even scrolling some more to find that one feature that I needed to quickly modify.  By having folders you can shorten up that tree and eliminate all of that time wasting scrolling.

4 Quick & Simple Uses

Move Subassemblies – Move a solo or group of subassemblies inside your master assembly.  If you are like me and use subassemblies from time to time you might have noticed that it can be a pain to move that subassembly up or down your FeatureTree.  By adding it/them to a folder you can move the whole folder, then delete the folder and your FeatureTree will be organized like you are hoping for.  Tip – another way to accomplish this is by holding down ALT while dragging a subassembly to relocate.

Group Common Parts – Do you have a whole pile of nuts and bolts scattered in your FeatureTree or maybe a mole hill of springs and pins.  Well if you have more than 1 of the same component in your assembly FeatureTree I would highly suggest throwing all of the common items in a folder and label the folder whatever you please.  I usually create a folder with all the components I drag in from our Design Library because these are non editable, no drawing files that need to be in the design.

Group Common Features – Just like the common part use this is a nice and easy way to quickly group all of your chamfers, radii or even reference geometry into a folder so that you don’t have to stare at its boringness during your entire design process.

Move Multiple Features at the Same Time – You may have seen this warning before about dragging multiple features all at one time.

Well by dropping them all in a folder you can move all of these features at one time with out having to move each one individually.  Can you say…time saving!

Closing Remarks

This option gives me that warm and fuzzy feeling when I finished up a model because I know my FeatureTree is nice and orderly.  Well on second thought, maybe that feeling is the burrito I had for lunch.

So do you use folders and if you do how do you use them?  Please drop me a comment and share what your experiences are with folders.

UPDATE:  Thanks to Brian from CADFanatic for pointing out a misprint of mine.  To move a subassembly in the FeatureTree without dropping it into another subassembly you need to hold down ALT to drag NOT Ctrl.  Sorry for the mistake.

As most of you know, the economy that we are in right now can be cut throat for most companies.  Any area that you can find to cut costs when submitting a quote need to be looked at because your competitors are.  In the industry that I work in, which is deep draw metal stamping, one of the big factors of cost are steel costs.  For those that are not familiar with metal stamping there is usually a fair amount of material that gets cut off and thrown away for each part that comes out of the press.  This unfortunately is just the nature of the industry but there are definitely some things that you can do to eliminate as much of this scrap as possible.  One of the things you want to do is make sure that you don’t have a bigger blank than what you actually need.  What is a blank you ask?  The blank is the pierce of steel, normally round in deep draw metal stamping, that you use to create your final part through a series of drawing, squaring, piercing, and trimming processes.

Before SolidWorks

Before our company made the giant step of purchasing SolidWorks we just used a 2D CAD package for all of our tooling designs.  The process of determining what size our blank should be for all new parts that we received was a well thought out spreadsheet formula that took many things into account and then spit out a blank size for us to use.  Well, more times than not, the blank that we had for these jobs came out much bigger than what we needed which resulted in either too much scrap being tossed out or the need to spend more money on tooling to make the blank sizes more accurate.

Using SolidWorks

The reason for our company to purchase SolidWorks was not really related to this at all but we soon found out that there were some tools available inside the software package that allowed us a more accurate size to start with.  Here is what we have developed as a company standard now for determining what size blank we should base our tooling off of.

1. The initial step consists of us modeling up the part (picture below) to match the customer print that we received.  Many times there are other important factors that the customer print provides us such as starting material thickness.
2. Next up we will want to fill in the pierce holes on the part (if it has any) and then add a ring to the top of the part that we can trim away to give a nice crisp edge.
3. From this part we can now use some SolidWorks functionality to help us out.  We now take this part and find out what the volume of the model is (Tools > Mass Properties > Volume).  This gives us a number that we would want our blank to match.
4. We now model up a blank (round disk, picture above) that is the thickness that our customer provided us on the print for starting material thickness.  Now by changing the diameter of the blank we can match this model’s volume to that of the volume that was determined in step 3.

This method has become for useful for us and gives us a very accurate number to base our blank size off of and there for the rest of the tool.

How About You

So here is what I am wondering.  How do you use the volume tool?  Do you use it at all?  By seeing something like this post do you think you have an application that you could begin using it for?

Drop me a comment and let me know.