Customizing QR codes

A couple of weeks ago I mentioned I'd be posting a video of how to take QR martix codes to the next level by customizing them with GIMP. Gimp is a free open source image editing software similar to Photoshop.

Cheers

Bob McGaughey, CSWE

CATI

How to Insert Dowel Pin Holes in SolidWorks

Many SolidWorks users, especially woodworkers, have asked for this enhancement for awhile: Have the ability to define a hole as a dowel pin hole in the part and have it automatically insert a dowel pin symbol in the drawing.

Starting in SolidWorks 2013, users now have the ability to add dowel pin holes. (Applause!) Dowel holes are used to align components in assemblies. Standard dowel holes have been added to SolidWorks in the Hole Wizard. So, all you need to do now is to click on Hole Wizard.  In the Hole Specification PropertyManager, on the Type tab, click the Hole button under Hole Type. In Type, select Dowels. SolidWorks gives you standard diameters to choose from or you can assign custom diameters appropriate to your industry. Fit options are also available. Set options as needed. That’s it!

Now that we have added dowel holes to the SolidWorks part document, let’s take a look at the drawing. There is a new document option for the automatic creation of all dowel pin symbols on view creation. Go to Tools > Options. On the Document Properties tab, click Detailing. Under Auto insert on view creation, you can select either Dowel symbols -part or Dowel symbols -assembly. Then, click OK.

Additionally, you can automatically insert all dowel pin symbols in a SolidWorks drawing view after view creation. You can automatically insert dowel pin symbols for dowel holes created with the Hole Wizard. To automatically insert dowel pin symbols into a drawing, pull down the Insert menu and pick Annotations > Dowel Pin Symbol. Under Auto Insert, select For all dowel holes.

As you select the drawing views, the dowel pin symbols are inserted in the view. Note that you have the ability to flip a dowel pin symbol after it has been inserted (right-click the symbol and click Flip Symbol.)

Lastly, to manually insert dowel pin symbols into a SolidWorks drawing, pull down the Insert menu and pick Annotations > Dowel Pin Symbol. Select a circular edge, a sketched circle, or an arc. Note that you can pre-select your circular edges, sketched circles, or arcs and then click Insert > Annotations > Dowel Pin Symbol. Dowel pin symbols appear in the selected holes.

Although this Dowel pin feature in SolidWorks is great, there are some improvements already requested like:

The ability to define a dowel pin hole tolerance by either the hole or the pin.
Add functionality to insert dowel pins
Ability to add Dowel Pin symbol to a point, not just circular edge or arc

Neil Bucalo
Certified SolidWorks Support
Technician 2013 Computer Aided Technology, Inc.

What's new in Solidworks 2013 - Center of Mass

Display Center of
Mass in a drawing 

New in Solidworks 2103, you can now display and dimension to
the Center of Mass in a drawing.

To do this, you must first insert the Center of Mass into
your model/assy.

Select Insert reference geometry/Center of mass. The center
of mass will now be displayed on in your part.

This can now be used in your drawing to dimension to;
however you must first display it in the drawing view: - Insert/Model Items/Reference
Items –select Center of Mass.

Mirror, Mirror, Where's my sheet metal notes?

So many of us have had the opportunity to make mirrored sheet metal parts. Over the years the process has changed and we are pretty close to having it all. However we still see a snag here and there with the drawings for these neat tools.

On the mirrored sheet metal part, if you choose to keep the link in the model you can't get your notes on the drawing. If you break the link you can get all your features and then create a new flat blank, but then it's not updating on it's own. So what can we do?

I have created a workaround mirrored sheet metal part to make both updating and sheet metal notes work on the drawings.

Since the sheet metal notes are created with the flat pattern view we need to have 2 of them. A good way to do this is to duplicate the sheet metal bodies and not the whole part.

Here we see the whole tree, let's break it down.

 

First we have rolled it back to look at our steps.

 

I created a mirror feature and chose the bodies to mirror option.

 

Then I deleted the initial body. (don't worry we get that back later)

 

I then created a derived configuration of the initial sheet metal part, this way the mirror will update when the initial body does. In the initial confiugration the mirror and the delete body are suppress. In the mirroed configuration the mirror and delete body are unsuppress. Then I used a drawing to insert a flat pattern of each configuration so that those flat patter configurations were created. The flats are important to get the sheet metal notes.

 

On the drawing you can now see all of the bent and flattened states of the part.

This may be a little on the long side but it works until the SPR is finished and we have the new controls to work with.

John Van Engen
CATI Tech Support

 

Where's the center of mass?

Recently I have had customers asking for a way to add a center of mass point to their drawing so they can dimension to this point.   This is now possible in SolidWorks 2013 using the Center of Mass function.

To use this function, you must turn on this function in your part or assembly.  To do so, go into the
mass properties window and check the option “Create Center of Mass Feature”.

This will create a Center of Mass feature in the Feature Tree just below the origin.

To access this point inside of your drawing file you will need to go to Insert, Model items and check the option for
Center of Mass under the Reference Geometry section.

You will now see the center of mass point on the drawing.  This can be dimension to, and will update as the model changes.

Hope this helps you out.

 

- Bryan Pawlak, CSWE

 CATI

Free SolidWorks from Performance Constraints (FSWPC-13-#21)

Optimal Configuration & Conclusion

In looking back at the past 20 articles we have posted about Free SolidWorks from Performance Constrains one of the items we promised in our first article was to give you the two optimal configurations that gave us the best overall performance.

Before we get to the results lets recap what we tested in our previous articles:

• RAM
  


• Processor Clock Speed
  


• Number of Cores and SolidWorks
  


• Hard Drive Speed
  


• Graphics Cards
  


• SolidWorks files stored in an older version
  


• Windows Visual Settings
  


• SolidWorks Options Set to Optimal
  


• SolidWorks Image Quality
  


• SolidWorks RealView Graphics
  


• Level of Detail in Parts and Assemblies
  


• Reducing Top Level Mates and Solving Subassemblies as Rigid
  


• Defeature
  


• Envelope
  


• Large Design Review
  


• SpeedPak
  


• Save Assembly as Part (3 options)
  


• Large Assembly Mode & Lightweight
  

In the list above you want to take note that of the 18 items we tested 13 of them are FREE.

The first scenario that we tested included all of the performance improvements explained above except Large Assembly Mode and Lightweight options. The environment looked like this:

Typical and Practical Hardware configurations

Configuration

• SolidWorks Options Optimized
  


• OS visuals set to best performance
  

Modeling methods

• Level of detail reduced
  


• Image quality reduced
  


• Realview Graphics off
  


• Top level mates reduced
  

In our first test the combination of the enhancements to our SolidWorks environment yielded some impressive performance results.

If we take all of the settings and hardware listed above and add in Large Assembly Mode and Lightweight we can see that it has even more of an impact in our results.

You can by looking at our deltas see that on our Practical machine we gained over 76% total improvement taking our benchmark run time down to just over 18min. If we look at the Typical machine we can see that the overall improvement is almost a 90% performance gain and our benchmark run time has gone from 4:43:44 to 0:28:50.

Conclusion

What we have found in our efforts conducting these tests is that improvement of a modeling environment must be approached at a system level rather than a specific component level. All of the hardware, configuration, and modeling methodology options work in concert to establish the performance capabilities of a workstation whether it's good or bad. Adding more processor power to a workstation that is short on RAM will help. But the improvement that the stronger processor yields will be much greater if RAM is added as well.

Understanding these several aspects of a SolidWorks modeling environment and how they work together can make all the difference in ensuring that you get the full value from your hardware and software purchase.

Adrian and I plan on continuing our testing for the next SolidWorks World in 2014 so please keep checking back for updates. We are planning on creating some new tests and new ways to display the results. If you have any suggestions please add a comment to this or any of our other articles.

Please
check back to the CATI blog as we will continue posting our
series of articles that goes further into the details of each of our tests. All
of these articles will be stored in the category of Free SolidWorks from Performance
Constraints and links to each with their
release date are listed below:

• FSWPC-13-#1 Introduction (3/19/13)


• FSWPC-13-#2 RAM (3/21/13)


• FSWPC-13-#3 Processor Cores (3/26/13)


• FSWPC-13-#4 Processor Cores for Simulation
  and PhotoView360 (3/28/13)


• FSWPC-13-#5 Processor Clock Speed (4/2/13)


• FSWPC-13-#6 Hard Drives (4/4/13)


• FSWPC-13-#7a Graphics Cards-SolidWorks
  Functionality (4/9/13)


• FSWPC-13-#7b Graphics Cards-Hardware
  Comparison (4/11/13)


• FSWPC-13-#7c Graphics Cards-Model Complexity (4/16/13)


• FSWPC-13-#8 Files stored in an older version
  (4/18/13)


• FSWPC-13-#9 OS Visual and User Settings (4/23/13)


• FSWPC-13-#10 SolidWorks Options (4/25/13)


• FSWPC-13-#11 SolidWorks Image Quality (4/30/13)


• FSWPC-13-#12 SolidWorks RealView Graphics (5/2/13)


• FSWPC-13-#13 SolidWorks  Level of Detail (5/7/13)


• FSWPC-13-#14 SolidWorks Mates and Flexible
  Subassemblies (5/9/13)


• FSWPC-13-#15 SolidWorks Defeature (5/14/13)


• FSWPC-13-#16 SolidWorks Envelope (5/16/13)


• FSWPC-13-#17 SolidWorks Large
  Design Review (5/21/13)


• FSWPC-13-#18 SolidWorks
  SpeedPak (5/23/13)


• FSWPC-13-#19 SolidWorks Save as Part (5/28/13)


• FSWPC-13-#20 SolidWorks Large Assembly Mode (5/30/13)


• FSWPC-13-#21 Optimal Configuration and
  Conclusion (6/4/13)

Thanks,

Josh
Altergott, CATI Support Manager

Adrian
Fanjoy, CATI Technical Services Director

 

 

FeatureManager Design Tree "Flat Tree" option - New for SolidWorks 2013

SolidWorks 2013 has 2 new FeatureManager Design Tree features. In my May Blog, I highlighted the Feature Manager Design Tree "Favorites" option. The second new feature is the Feature Manager Design Flat Tree option.

The FeatureManager Design Tree View allows
the user to show a "Flat Tree" option. a Flat Tree is where the
features are shown in the order they were created, instead of hierarchically.
In a flat view, curves, 2D sketches, 3D sketches are not absorbed into the
features that reference them.

Note: the Flat Tree View is only for parts and the following items
are unabsorbed in Flat Tree View:

• Simple
  hole


• Hole
  Wizard holes


• Mounting
  boss


• Lip/Groove


• Snap
  hook groove


• Vent


• Snap
  hook


• Vent


• Snap
  hook


• Sheet
  metal feature


• Library
  feature


• Weldment
  structural member


• Sketch
  block

Here's how it works:

Right mouse click on the part name in the FeatureManager DesignTree. In the pull down menu, go to Tree Display and click on Show Flat Tree View.

Below is the FeatureManager Design tree using the Flat Tree option:

Notice that the sketches are not absorbed under their associated feature; sketches and features are now in the order in which the model was built. This tree option can be toggled on and off at any time. 

Thanks!

Judy Marlo

Application Engineer

CATI St. Louis