Did you miss it? SolidWorks World 2011! I did

 

Just like you, I was unable to attend this year's wonderful SolidWorks World Conference in sunny San Antonio, TX. Someone had to hold down the fort, although it would have been nice to meet Kevin Bacon. If your thirst for SolidWorks is great, well you are in luck. All the breakout sessions, which are jammed pack with info, are available from SolidWorks World 2009, 2010 & 2011. So if you missed my presentation at 2010 SWW, you can get that too. That and check out the list that our tech team gave this year.

Drawings: Template & Sheet Format Setup	Jim Krivoshein
How to Prepare for Your Enterprise PDM Implementation	Justin Webster
Redneck Workarounds: Creative Solutions to Everyday Problems	Todd Werginz and Josh Altergott
DriveWorksXpress Hands-on Test Drive	Jake Smith
Maximizing SolidWorks' Performance	Adrian Fanjoy and Josh Altergott
Design-Tables the Complete Story: How to Build and Maintain Effective Design-Tables	Josh Altergott
Preparation of Imported Geometry for Molding	Todd Werginz
The World is Non Linear	Rajat Trehan

SolidWorks World Presentations 

 



Bob McGaughey, CSWE

Solution Technical Manager

CATI

“Normal To” Orientation.

Sometimes, when rotating “Normal To” a face, the orientation can be rotated at some obscure angle.  This can be especially true on imported parts or parts that have a lot of funky angles to them.  Take a look at this part.  When you rotate the selected face Normal To, you get the following results…

 

If you want to rotate the part with respect to a specific face, simply ctrl + select the two faces before selecting Normal To.  The face that is selected second will automatically be rotated to the top.

 

Final rotation result…

 

 

For more rotation solutions, please see the blog articles below…

http://blog.cati.com/2011/02/how-to-change-the-orientation-of-an-imported-solidworks-part.html

http://blog.cati.com/2011/02/how-to-change-orientation-of-an-existing-solidworks-part.html

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Sketch Picture

Say you have a picture of what you want to create in SolidWorks and instead of guessing at the outline, you want to trace it off of the picture instead. No problem, to insert a 2D picture into a SolidWorks part to trace, follow the instructions below.

1.  Select the plane on which you would like to create the outline.


2.  Open the sketch.


3.  Inside of the sketch go to tools --> sketch tools --> sketch picture.


4. Select the picture that you would like to insert (File types that you can use for these pictures include .bmp, .gif, .jpg, .jpeg, .tiff, or .wmf.)


5. Start sketching!

 Courtney Freeland

Technical Analyst

Computer Aided Technology

Turning Off Add-ins (MSWP#4)

This article continues our Maximizing SolidWorks Performance series.  If you would like a little background information please refer to the first article in the series Maximizing SolidWorks Performance (Results).

Everything running on your computer takes some amount of resources.  I mean everything.  Right down to the insignificant little app that tell you when the Adobe Acrobat Reader has an ungrade available.  It is recommended to reduced the amount of applications, programs, apps, widgets, and add-ins running on your computer to increase performance as much as possible. 

In our case we ran our baseline with several Add-ins for SolidWorks activated.  Each of these add-ins take a little bit of RAM leaving a little less for the operations that we are actually using in the benchmark.  The add-ins that we had turned on in our baseline were:

• Photoview 360


• SolidWorks Simulation


• SolidWorks Toolbox


• SolidWorks Toolbox Browser


• SolidWorks Utilities

In this test we turned off all Add-ins and got the following results::

 
The chart above shows that freeing up even a relatively small amount of resources can have a noticeable difference in performance and in our specific case it sped up SolidWorks in every category we measured.

Results:

• Rotations 13% faster saving ~4mins


• Modeling 31% faster saving ~22 ½ mins


• Closing 17% faster saving ~9 ½ mins

Total:

• 9% faster saving ~44 mins

Other ways of freeing up resources include:

• Removing non-essential applets (weather bug, chat tools, external email notifiers, etc...)


• Trade listening to music on your computer for buying a dock for your iPOD


• use Autoruns to find and deactivate unnecessary services that run automatically (for advanced users)


• Turn off all non-essential programs that may be running on the desktop

All of these helpful little programs pull resources that otherwise SolidWorks may use.  The best rule of thumb would be to "focus your computers power on what is most important to you".

Adrian Fanjoy

Technical Services Director

Computer Aided Technology, Inc.

Justifying sketch text.

The trick to justifying sketch text starts before you open the sketch text command. You will need to draw in a construction line or have a line in the sketch to use. If the sketch text command is opened it will not let you use the other sketch tools, so the line must exist first. Once that is done, start your sketch text command, write your text, select a font, and choose the construction line.

John Van Engen

CATI Tech Support

 

Solidworks SP 3.0 is Live!!

Solidworks service pack 3.0 is live for download as of 3/23/11. Both 32 bit and 64 bit platforms are available for download.

 

SolidWorks 2011 SP3.0

 

Todd Werginz

Technical Ananlyst

CATI

 

Reference File Locations (MSWP#3)

This article continues our Maximizing SolidWorks Performance series.  If you would like a little background information please refer to the first article in the series Maximizing SolidWorks Performance (Results).

This article is describing one of our "side tests".  Some of our tests, including this one, while being run with the same methodology as all of the others did not fit the general flow of the over all testing.  This test was run to show the negative impact of a seldom used system option (reference file locations) that can have dire consequences.

The good new about reference file locations is that most people are not using them and those who are using them are generally using them correctly.  This was a much more prolific problem a few years ago.  Reference file locations is a way to help ensure that SolidWorks is going to find the files that it needs for a particular assembly that might be stored other locations in an environment usually a network location.  When an assembly opens and the Search file locations for external references option is checked, SolidWorks searches all of the folder in the reference documents list as set in System options|File locations.

 
 
 
While in our specific environment the detrimental affect on performance was not huge, I have seen this situation affect customers to the point of paralysis. 

 
Results:

• Opens 22% slower costing ~3 ½mins


• Rebuilds 14% slower costing ~21mins


• Switching sheets 20% slower costing ~11mins


• Saves 13% slower costing ~8mins


• Modeling 23% faster saving ~16 ½ mins

 Total:

• 6% slower costing ~29mins

The most important thing to notice about these results is that the modeling sections ran 23% faster than the baseline.  If you think about this you will probably come up with the same conclusion I did.  There is no reason to believe that that is real.  There is no reason that the modeling sections should have been affected in the least by these system option.  I believe that this must have been some kind of fluke in our testing.  All of the other results are just as we would have expected; or at least, within a reasonable margin of error.

The key here is to remember that the reference file locations options should be used in very special circumstances and your VAR should be contacted to discuss all of your options. If there are alternatives that allow you to avoid this course they can assist you in finding them.

Adrian Fanjoy

Technical Services Director

Computer Aided Technology, Inc.

 

How to set a Sub-Assembly to Flexible in a SolidWorks Assembly

In going through our support log this week I saw a question that had come up a couple of times and that was “How to set a sub-assembly so that its movement could be reused in an upper level assembly?”

By default all assemblies when inserted into another assembly are set to rigid, meaning the sub-assembly acts as a single unit and its components do not move relative to each other. If you want to be able to reuse that sub-assemblies movement in an upper level assembly you can do this by setting the properties of that sub-assembly to Flexible by:

1. Left or Right clicking on the Sub-Assembly in the Feature Tree.


2. Selecting the Component Properties icon.


3. In the Component Properties dialog box set the Solve as to Flexible.

 
When a sub-assembly has been set to Flexible the icon will change to  to indicate the status of the sub-assembly.

Please note the following regarding flexible sub-assemblies:

• Mates. The mates in a flexible sub-assembly are solved simultaneously with the mates of the parent assembly. Therefore, moving or rotating a sub-assembly component does not violate the mates in the sub-assembly or its parent. A component moves only within its degrees of freedom according to its mates. Also because mates are being solved for multiple assemblies this can increase rebuild times and effect the overall performance of your assembly.


• Multiple Instances. You can insert more than one instance of the sub-assembly in the same configuration of the parent assembly. You can make some instances rigid and others flexible and the different instances can have different positions of the sub-assembly components.

Josh Altergott

CATI Tech Support

 

SolidWorks System Options Set to Optimal (MSWP#2)

So I couldn't wait to get started.  As soon as I published the introduction to this series I wanted to at least get the first article out so that everyone could get an idea of what to expect.

In this test we compared SolidWorks system options that we typically see (and did see with the customers that gave us our test models) with what we consider optimal for working with an assembly this large.  To remind yourself of the details -- http://blog.cati.com/2011/03/maximizing-solidworks-performance-results.html.  The results of this are shown below:

 
Results:

•Opens 39% faster saving ~15 ½ mins

•Switching Sheets 15% faster saving ~8 ½ mins

•Closes 9% faster saving ~5mins

Total:

•7% faster saving ~32 ½ mins

Now, it wouldn't be fair to tell you that you could potentially save 7% and not tell you what the settings are that we consider optimal.  So here they are:

    
 
 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

In our opinion, each of these settings allows the user to potentially improve performance by saving system resources so that RAM and Processor power can be better directed to more productive aspects of SolidWorks.  Most of the settings that have been changed let the user work in a "prettier" environment.  Please remember that the prettier it is the slower it is.

Also note that a 7% speed improvement is nothing to sneeze at and it only gets better from here.  We are publishing these in order of least to most impressive.

Adrian Fanjoy

Technical Services Director

Computer Aided Technology, Inc.

Maximizing SolidWorks Performance (Results)

As many of you may know Josh Altergott and I did a presentation at SolidWorks World this year in San Antonio titled "Maximizing SolidWorks Performance".  The presentation was well received and we thought it would be a good idea to share the information with more than just the SolidWorks World attendees.

 The goal of this presentation was to determine the most effective changes that could be made to a SolidWorks environment and to SolidWorks modeling methods in the hopes of improving the performance of the software.  This link will take you to an article that describes our premise in a little more detail.  http://blog.cati.com/2011/01/maximizing-solidworks-performance.html.  Basically, we wanted to see what makes SolidWorks move faster and prove it.

To determine what makes SolidWorks perform we had to test each individual item "individually".  The process we used to accomplish this follows:

• We ran a baseline test with the machine, the OS, the model, and SolidWorks all setup in a specific manner.  That test took ~7hrs and 50mins to run.


• Next we changed one item. (ie. we changed our SolidWorks system options to what we believed to be the optimal)


• We then ran the exact same test and measured the difference.


• After that we would set everything back to the baseline and change something different.


• Again and again until we checked everything we could.

The Base line

In our experiment it was required to have a fixed point of comparison.  Our baseline configuration is described as Beaker2011.  (You may remember Beaker as the hapless assistant to Dr. Bunsen Honeydew in the Muppet Labs sketch on the Muppet Show in the late 70's and early 80's.  http://muppet.wikia.com/wiki/Beaker). We abused our Beaker almost as heanously as Dr. honeydew abused the original.  Here's how our baaseline was configured:

The Model

• The model is a conglomeration of several models that were brought to us by customers because performance was lacking.


• The directory that holds the model is 2.4GB


• 6637 total components


• 5862 parts


• 775 sub assemblies


• 663 top level mates


• 13011 bodies

The machine

• Dell T5500


• 1 - 2.4Ghz processor running 2 cores


• 6 GB RAM


• Windows 7 64bit OS


• Nvidia Quadro Fx 4000 Video card


• SolidWorks 2011 SP1.0


• 1 - 1TB 7200 RPM drive for storage


• 3 - 320 GB 7200 RPM drives RAID 0 for the OS

 

The environment

• File stored in the current version


• Files stored locally


• Swap set to OS default


• Storage on a single disk


• Assembly is fully resolved


• SolidWorks system options set to defaults


• Several Add-ins turned on


• RealView Graphics turned on


• Image quality set high


• OS and user settings set to defaults


• High level of detail in purchased parts

In our tests we run the same macro each time.  It puts the model through a series of modeling changes, view changes, rebuilds, etc... to not only show how much of a performance increase (or decrease) we can get but also where we can expect to see that difference (ie. modeling, rotations, rebuilds, opens, closes, saves, etc...)  When our baseline ran we saw these results:

All of our tests are compared to this graph.  The Y axis of this graph is total time spent doing these operations measured in seconds.

In the subsequent articles in this series we are going to explore each test that we did starting with the change that produced the least amount of improvement to SolidWorks performance and continuing through the change that produced the largest amount of benefit.  We will finish with 2 optimal configurations to see what the effect can be when you combine all of these improvements together into the same environment and model set.  Occasionally we will veer off track and discuss a side topic here and there as well.

It is also important to realize that the results that we found in our tests are specific to our model, environment, configuration, and even the phase of the moon.  Results that you see may be slightly or extremely different.  We worked very hard to make this produce results that will give, at least a ball park idea of what can be expected elsewhere, but realizing that we cannot determine what other environment may hold, we will not garauntee the effect these changes will have in any environment other than ours.

I hope you find these articles informative and helpful.

Adrian Fanjoy

Why is there two origins in a sketch; one red, one blue?

 
When editing any sketch one can see two origins; one red and one blue.  The blue origin is always there but hidden if you have it set to that.  It’s the center of the part file and never changes orientation from the triad in the bottom left hand corner.  The red origin changes orientation depending on how your sketch plane is created.  Just as the sketch geometry is read by solidworks in polar coordinate the planes are also orientated in them.  For instance in the picture below I have created an offset plane some distance from the front plane.  The Y-Axis is pointing up and the X-Axis pointing to the right just as the traid in the bottom left corner shows.

 

Ketul

CATI Support

ISOMETRIC BROKEN OUT SECTION WITH CROP

        I had a question come up the other day with a cropped view. The customer was asking for a broken out section, (which BTW is an Awesome feature in Solidworks!) He had already cropped the view because it was a 95' long part and that did not look to good on the sheet. He was looking to get inside and show off
some of the componentry in the detail if you will. The problem is that this a current limitation in an Isometric view. So how do you work around this you ask???? Well I came up with this- in the assembly you can do a spline on a plane normal to the view you want to cut.

        I created a configuration at the assembly level called cutaway and sketched a spline at the assembly level.  I was able to control which parts it affected and if I wanted it to propagate back to parts. (No not really)

            So in the view it ends up looking like this after picking the correct configuration. All that is left is to use the break command from the View Layout toolbar on the command manager.

 

 

 

 

 

 

 

 

 

 

 

 

 

Todd Werginz, Technical Analyst

CATI

Shortcut Bar AKA the "S" key

SolidWorks has really put in a lot of effort in the past couple of releases to minimize mouse travel and increase productivity.  One of the tools that they have added to help do this is the shortcut bar.  This shortcut bar is basically a tool bar that can be pulled up by hitting the “s” key on the keyboard.  It opens up right beside your curser eliminating the need to drag your mouse to the top command manager.  The best part about it, it’s completely customizable.  It is also context sensitive and can be pulled up in parts, assemblies and drawings.  Depending on what mode you are in, it can be modified to suit your modeling practices.  

To modify this shortcut bar, you need to first pull it up.  The “s” key is the default key to do this.  Once it is active, simply right-click on the toolbar.  The only option you get is “customize”.  Notice that it is the same menu you use to customize all other toolbars.  Simply drag the icons you wish to add onto the toolbar.  If you don’t like the default “s” key to bring up the shortcut bar, this too can be customized.  Go to the keyboard tab and search for “shortcut”.

 

Below is a screen shot of what mine looks like in sketch mode.  Because you can extrude directly from a sketch, I have added the extrude boss and cut icons among others.  Notice that the extrude cut icon is grayed out.  Just like the normal toolbars, SW will automatically gray out features that are unavailable.

 

Another shot of the shortcut bar in part mode…

 

Now go out and customize your "s" key...

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Save SolidWorks Settings

If you are a user that likes to customize your version of SolidWorks, a simple way to maintain your settings when switching from one version of SolidWorks to the next is to use the Copy Settings Wizard. What this wizard does is it saves your system settings for keyboard shortcuts, menu customizations, toolbar layouts (all or Macro toolbar only), as well as your system options. To backup your settings please follow the instructions below.

When saving your system settings you can either have SolidWorks open or closed, however if you have SolidWorks open the settings in the current session are not saved.

1.)     In Windows, go to Start, All Programs, SolidWorks 20XX, the SolidWorks Tools folder, and finally Copy Settings Wizard as shown below.

    

2.)    Select Save Settings and click on the next button.

3.)    Browse to a location and file name of where you want to save your settings to, select the type of settings that you would like to save and then click on finish.

4.)    Click OK.

 

To restore your settings first make sure that there is not a session of SolidWorks running.

1.)    Go back to the SolidWorks Copy Settings Wizard and this time select restore settings.

2.)    Browse to the file in which you saved your setting and select the types of settings that you would like to restore, click next.

3.)    Select the type of destination (Current user, One or more network computers, or one or more roaming user profiles) then click on Next.

If you selected:

-Current user – go to next step

   -One or more network computers - a list of available computers is displayed

   -One or more roaming user profiles - a list of available users is displayed

4.)  Select a user or a computer and click Add, repeat until you have specified all comptuter’s or users, then click Next.

5.)  Slecet or clear Create backup of current settings for (each computer/user), then click Finish.

6.)  Click OK.

 

Courtney Freeland

Technical Analyst

Computer Aided Technology

How to submit a SolidWorks Enhancement Request

About a week and half ago I posted a article on how to remove the locks from the SolidWorks Customer Portal (http://blog.cati.com/2011/03/how-to-remove-the-locks-in-the-solidworks-customer-portal.html) so I thought it would be good to follow it up with how to submit a SolidWorks Enhancement Request.  So to put in an Enhancement Request you will need to do the following:

1. Log in to the SolidWorks Customer Portal (https://login.solidworks.com/nidp/idff/sso?id=cpenglish&sid=2&option=credential&sid=2)


2. Select the Enhancement Request link.
    


3. Search to see if there has been a similar request before.
    


4. If none of the results match yours then select the link at the bottom of the page and generate a new Enhancement Request.

           
Your Enhancement Request will be assigned a number and you will receive a confirmation from SolidWorks stating that their request was received. 

Enhancement Requests are tracked and put into production based on the requests submitted by customers via the Customer Portal.  If multiple customers show interest in seeing the same product enhancement, then the SolidWorks Developers will focus on adding that enhancement to the next release.  Requests need to be submitted by the customer through the Customer Portal in order to make issues visible to SolidWorks Developers.

Here is the link to the Enhancement Request form:  http://www.solidworks.com/pages/services/subscription/Enhancements.html

Josh Altergott

CATI Support Team Leader

Mechatronics and Machine Design Seminar: SolidWorks and Motion Analyzer

Attention Machine Designers!

Join CATI and Revere Electric for this exciting seminar to see how you can improve your machine design process with SolidWorks and Motion Analyzer.

Motion Analyzer, from Rockwell Automation, used in conjunction with SolidWorks offers design engineers virtual prototyping. This prototyping reduces the time to design, develop, and deliver.

>View Agenda and Register

Mechatronic design is a collaborative venture between mechanical, electrical, and control design engineers – the outcome is a machine design optimized for high performance controls.

When:
Friday, April 15th, 2011
8:00 am - 1:00 pm CST

Where:
Revere Electric
Buffalo Grove Office
975 Weiland Road
Buffalo Grove, IL 60089

>View Agenda and Register

Hope to see you there!

 

Jim TeDesco
Marketing
Computer AIded Technology, Inc.

Why is there a Funnel next to my Selection Pointer?

Everyone has at some point in time been working in SolidWorks when you realize that you are no longer able to select what you want and that is when you notice the Funnel next to your Selection Pointer. So what is that funnel and how did it get there? 

What this Funnel is is a Selection Filter and is used to help select specific types of items in the graphics area or drawing sheet. This more than likely got turned on by accidentally selecting one of the Hot Keys on the keyboard. There are 3 Hot Keys or Keyboard Shortcuts assigned to Selection Filters E for Edges, F for Faces, and V for Vertices. You can access the full Tool Bar by Right Clicking on any of the existing Toolbars and selecting the Selection Filter Toolbar or by hitting F5 on the keyboard.

 
If you are looking for a fast way to turn off or Clear All Filters you can hit F6 on the keyboard.

Josh Altergott

CATI Support Team Leader

How to Copy a Part in an Assembly with Mates

So you have an assembly and have been given the task of inserting multiple copies of the same part into it. The question then becomes what is the fastest way to create all of these instances and have them properly mated into position. As with most tasks in SolidWorks there is always more than one way to get the job done.

The first is if you are going to use the part file on a continuous basis then you can utilize Mate References. Mate References are found in the Reference Geometry Sub Menu on the Features Toolbar. In the Mate Reference property manager you specify different geometry for the First, Second, and Tertiary Mate. For each mate you can specify a specific Mate type based upon the selection or go with the default. You can also specify a Mate Alignment for each mate as well. Generally you will then want to add you file with it Mate Reference to the SolidWorks Design Library so that it can be used again just by dragging and dropping from the Design Library.

 

 

The second option is the one I personally use the most and that is Copy with Mates command which can be accessed through the Insert Components sub menu from the Assembly Toolbar. This is very easy to use, it gives you the ability to Repeat if the Mate is going to be same, Flip Alignment and even change distance or angle depending on the mate type you select. This a great option if you have more than one of an item to insert into your assembly.

Josh Altergott

CATI Support Team Leader

What Does the License Count Mean in the SolidNetwork License Administrator?

Every time someone new works on their companies SolidWorks Network License Administrator for the first time we usually get the support call asking why the license count in the License Administrator is different than what they actually own.

 
If we take a look at an example from one of our customers you will see that the license count for Standard SolidWorks is 67 seats but in the SNL Admin it show that they have 98 Standard SolidWorks seats listed. This is because the customer really owns 67 Standard, 2 Office, 7 Professional, and 22 Premium seats and if you add all that up it equals 98 seats. How the SNL Admin works is that is breaks down the each of the seats that is a higher level than Standard into 2 seats (1 Standard and 1 with additional features) by breaking down the licenses it allows all users equal access to the functionality of the higher level seats. So when you start SolidWorks in the morning and have no Add-Ins turned on you get the Standard SolidWorks to start with then at some time later in the day you need to add some hardware to an assembly so you turn on SolidWorks Toolbox it will now go out to the server and pull the next license that is available whether it be Office (no longer available for purchase), Professional, or Premium.

You have the ability to control the order in which the licenses are distributed from the SNL Administrator and you also have the ability to create an options file that will control what users do/do not have access to the different types of SolidWorks.

Josh Altergott

CATI Support Team Leader

2011 SP3.0 Early Visibility

Solidworks is in early visibility for service pack 3.0 as of today. Both versions are availble X32 and X64.

 

Todd Werginz

Technical Analyst

Computer Aided Technology

Why are there different Sketch icons in my Feature Tree?

Today’s question from the support log is “Why are there different Sketch icons in my Feature Tree?”

The original support call we received the customer was only asking about 2 specific icons that they saw but for this article I thought I would expand on all the different icon symbols that you could see in the Feature Tree for a part file.

First up is the state of a sketch:

• (+) - Over Defined


• (–) - Under Defined


• (?) - The sketch could not be solved


• No prefix - Fully Defined

With any of these Sketch states you may also see a second sketch icon that has a polygon and included circle. This indicates that one has used "Sketch Contours" for a feature. Sketch Contours are a means to use parts of a sketch (region(s)/boundaries) to create a feature.

Next up are the Errors and Warnings that are displayed next to part, feature, or sketch icons and described in tooltips (when the pointer hovers over the item) and in the What's Wrong? Dialog box.

•  - An error in the model


•  - An error with the feature


•  - A warning underneath the node


•  - A warning with the feature

The last item is the state of External References that are displayed next to part, feature, or sketch icons:

• If a part or feature has an external reference, its name is followed by –>. The name of any feature with external references is also followed by –>.


• If an external reference is currently out of context, the feature name and the part name are followed by ->?


• The suffix ->* means that the reference is locked.


• The suffix ->x means that the reference is broken.

Josh Altergott

CATI Support Team Leader