Hide / Show Components Quickly in SolidWorks 2012

3DVision TechnologiesToday, Josh Spencer from 3DVision Technology posted an awesome reminder/tip of a new feature that is included in SolidWorks 2012 on the 3DVision Technologies Blog.

In SolidWorks 2012, you now have the ability to quickly hide components using the “Tab” key and to quickly show components using “Shift + Tab”.  This is a feature that SolidWorks users fell in love with while using 3DVIA Composer.

In order to give credit where it is due,  please check out Josh’s blog post here on how this new feature really works!

RockSolid Tips & Tricks: Macro Shortcuts

Note:  A special thanks to Deepak Gupta, Filipe Venceslau, & Wayne Matus for answering my question on the SolidWorks Forums and for providing me the content for this blog post.

Did you just write that SolidWorks Macro that will solve ALL of the world’s problems?  I recently wrote one (with help) that will not solve ALL of the world’s problems but at least it will solve 1 of mine.

However, if you are at all like me, I am a keyboard shortcut kind of guy so that I can keep my UI as clean as possible. So there in lies the problem.  I wrote this super awesome macro but I didn’t really want to have a button on a toolbar that was only there so that I could assign a keyboard shortcut to it (see the normal macro button dialog box below).

Macro Button Dialog

So I asked the question on my original SolidWorks Forums Discussion if it was possible to assign a keyboard shortcut WITHOUT having to add a button and I was really happy to see that I could so here is how to do it (thanks to Wayne Matus).

So how would you go about doing this?  Well, here you go and it is ACTUALLY extremely simple.

1.  Create a folder called “Macros” in your SolidWorks install directory which is by default C:\Program Files\SolidWorks Corp\SolidWorks.  You will notice that the address in the picture below is set to C:\Program Files\SolidWorks 2011\SolidWorks which I like to do in the case that I have multiple versions of SolidWorks installed on my computer (which I normally do).

Add Macros Folder

2.  Copy all of your macros (or only the ones that you will want to assign keyboard shortcuts too) into your new folder

3.  Now if you go to add a keyboard shortcut (Tools > Customize > Keyboard tab) you will be able to select “Macros” from the Category dropdown.  From there you will be able to assign a shortcut as you would with any other command.

Keyboard Macros

I hope you find that as useful as I did.  Enjoy!

RockSolid Tips & Tricks: Mid Surface

This post was driven by a request that I had on one of the presentations I did earlier this year at a user group meeting.  I first saw this “trick” performed while watching the infamous Tips & Tricks Presentation that Phil Sluder does every year at SolidWorks World.

The SolidWorks Mid Surface tool is a tool that probably does not get used very often or probably more accurately has its really “specific” uses that are determined by each user.  However, I believe the example below would have a more wide spread use by more users.

Below you will notice and extruded rod that will built off of the origin.  The original sketch was created on the Front Plane but by not being on the origin it makes the other Planes unusable.  Now, you could create new reference geometry to use but for what we are trying to accomplish, I think the Mid Surface tool might be a better fit.

Beginning Model

1.  Begin by going to Insert > Surface > Mid Surface

Insert - Surface - Mid Surface

2.  Select both end faces.  Notice that when you select the 2nd face (as long as it is a valid selection), SolidWorks will automatically create a new Face Pair.

Mid Surface Tool

3.  Now you will want to hide the original Solid Body that you had so that only the Surface Body is showing.

4.  Now go to Insert > Surface > Extend

Insert - Surface - Extend

5.  Select your newly created surface and type in what kind of end condition you would like to have.  In the case of this, I am going to offset the surface by a Distance of .750in.  This will insure that no matter what size my initial rod is changed to, my surface will ALWAYS be .750in bigger.

Extend Surface Tool

6.  Now go to Insert > Boss / Base > Thicken

Insert - Boss Base - Thicken

7.  Again, select your surface, and thicken your surface by your desired amount.

Thicken Tool

In the picture below, I have highlighted the original dimensions from our model.  The length was originally drawn at 10.000in and the diameter was originally drawn at 2.000in.

Original Dimensions

Now, if you would happen to change the length of your rod, you will notice that everything maintains its relationships and stays perfectly centered.

Length Modification

Or if you change the diameter, you will notice that the offsets maintain their relationships.

Diameter Modification

BUT, probably my favorite reason for using this tool is that you can even change the original sketch shape (in the case below, to a square) and it maintains ALL of your relationships and spacing.

Shape Modification

Hopefully this post will trigger some ideas for you on how you can use this in a production environment.  Feel free to share how you currently use the Mid Surface tool or how you might use it in the future.  Also, feel free to drop a comment if you have any other questions about this tip.

hidden gem: total uninstall option now available

First and foremost, I am taking no credit for finding this so I want to give credit where credit is due.  Chris Snider, Application Engineer at 3DVision Technologies, posted a few weeks back on their blog that SolidWorks now has the “Total Uninstall” option that so many CAD Admins have begged and pleaded for for a long time.

However, this new option is not easily found unless you know where to look.  Starting with SolidWorks 2011 SP3.0, you can start the uninstall process, and click on the program bar at the top of the uninstall window as shown below.  From there you will notice the “Total Uninstall” option as shown below.

total uninstall

For more information on this you can check out the Forum Topic for this tool.

As a CAD Admin I want to personally thank the SolidWorks developers for finally adding this to the program.  This will make my life much, much, much simpler.

toolbox headaches in solidworks 2011? this might be the cause

headacheAre toolbox components making your head throb in SolidWorks 2011?

Well there is a new option that might be throwing you off and you probably aren’t even aware that it is checked by default out of the box.

In Tools > Options > Hole Wizard / Toolbox there is a new checkbox for a feature called “Make this folder the default search location for Toolbox components”.  According to the SolidWorks help file this new feature “is useful when you open models whose toolbox components do not reference your Toolbox folder. If you clear the system option, SolidWorks does not automatically search the Toolbox folder for references to Toolbox components.”

toolbox default search location

Whether this is the cause of your toolbox problems or not, the frustrating thing for me is that this option is checked by default out of the box.  I am not a huge fan of new features being added like this and it is automatically checked without being publicized in some way shape or form.  Unless you go through each option when a new release comes out (which I think every CAD Admin should) you probably wouldn’t have seen this or known about it.

wrapping text around a coned face

Have you ever had a coned surface that you needed to add text too?  I ran into this about a year ago and then came across the same situation this week again so I thought I would share with everyone here how I accomplished this.  I want to be upfront though, when I ran into this last year, Jeff Mirisola helped me out with how to accomplish this so I have to give him all of the credit for this.

Below you will see my original part.  Just a simple revolved part with a coned or angled face on it.

original body

Step 1

Your first step is to create a plane normal to the coned face.  Select the coned surface and then select a plane to make your new plane perpendicular to.  In my case I used the Right Plane.  SolidWorks will give you a result similar to what is shown below.

adding normal to plane

Step 2

On your newly created plane, start a new sketch and insert sketch Text.  You can find this at Tools > Sketch Entities > Text.  Positioning is kind of a science but I would suggest using some curves for your text to follow.  This is good for positioning as well as for making sure your text is centered.

add text

Step 3

Now you are ready to either emboss, deboss or scribe your text on your face.  Select the sketch you just created and then use the Wrap tool.  You can find this at Insert > Features > Wrap.  Now select the face that you want to wrap around, select whether you would like to emboss, deboss, or scribe and hit the green check mark.

wrap text

Voila!  You now have your text wrapped around your coned face as shown below.

final product

add a new hole type to the hole wizard

Have you ever wanted to add a hole type to the hole wizard in SolidWorks.  In a manufacturing environment you have common holes that you use such as reams or dowels.  Now you could just use the standard drill holes that are in the hole wizard BUT when you use the hole callout function in your drawings it will call them out as a drill and not a ream or a dowel.  This could pose huge problems for when you go to assemble your tool.  Here is a quick little way around that situation.

1.)  Go to Tools > Options > System Options > Hole Wizard / Toolbox and select Configure OR go to Start > All Programs > SolidWorks XXXX > SolidWorks Tools > Toolbox Settings.


2.)  Select and click on the standard that you would like to copy for your new standard.  It will more than likely be either ANSI Inch or ANSI Metric.


3.)  On the top of the screen you will notice an icon that will allow you to copy the standard.  Once you click on that button it will prompt you to name your new standard.  Name your new standard and select the green check mark.


4.)  If you have successfully completed this you will notice that SolidWorks is now creating a new standard.  In my case, I named my new standard “PRESS FIT DOWELS”.


5.)  Once it has been created, you will now notice it on your main screen with the rest of your standards.


6.)  Select your new standard and turn off everything that you do not want to keep.  In my case I am turning off everything but fractional drill holes.  You can see this in the next 3 images.






7.)  Once you have completed this, select option 2 on the top toolbar of your screen (next to the Save button).  Once you have moved to “2 – Customize Hardware” select your newly created standard.


8.)  Click through the necessary screens until you arrive at a screen that looks like below.  Now turn off all of the holes that you do not want to appear.  In my case I only want to be able to use a 1/4”, 5/16”, 3/8”, 7/16”, and a 1/2” press fit dowel.  Once you have turned off all of the ones you do not want to use, click Save and close the program.


9.)  Now you will want to find the calloutformat.txt file.  This is by default located at C:\Program Files\SolidWorks Corp\SolidWorks\lang\english.  Open the txt file and add a standard at the bottom.  To find out how to do this click here.  Save your calloutformat.txt file and close it.


10.)  Now open SolidWorks and start the hole wizard tool.  Click on the corresponding Hole Type icon which in my case is a drill hole and in the Standard dropdown, select your new standard.  You will notice that the sizes dropdown only include the hole sizes that you left checked.  Note:  Your new standard will only appear in the Standards dropdown on hole types that it has.


11.)  Now create a drawing of your part and using the Hole Callout function (located on the Annotation toolbar) dimension your holes.  You will see that the callout looks exactly like you called for in the calloutformat.txt file.


I hope this little trick will make your life easier and eliminate possible problems that you have currently come across.