CATI Tech Notes

Big Files = Big Problems

Think your part is way bigger than it should be? Maybe it is... Little known facts from 2011 SP2 there was an error that caused file size to balloon.

The problem was in the creation of multiple redundant display states that are all expendable. In 2011 SP3 the issue was corrected, however files with this issue will continue to have the issue. 2011 SP3 and later added a right mouse click menu to the display states called "purge redundant display states".

This will clean your file, and in some cases a lot. We saw a 200MB+ file go down to around 17MB. Big savings there.

Please make sure to back up your files before attempting this to make sure nothing undesirable happens to any wanted display states.

Happy Purging!!
John Van Engen
CATI Tech Support

Undo while in the power trim.

Afternoon everyone,

I learn something new everyday when it comes to SolidWorks, even after ten years of teach and demoing SolidWorks. Check out this one. Have you ever noticed when you do the power trim in the sketcher you get red boxes? Have you ever placed our cursor on the box and just kept trimming. Most of us just keep going. Well here is what are can do if you.... Whoops!!

Have a Great Day

Bob McGaughey, Certified SolidWorks Expert

CATI

Rolled Edge Flanges

A common feature in the sheet metal industry are rolled edge flanges on a cylindrical parts.  With all the great sheet metal tools that SolidWorks has to offer, that is one area the software has strugggled in the past.  SolidWorks has never had the capabilitys to create a part as such and still be able to create a flat pattern from it.  With the introduction of SolidWorks 2012, that has all changed.  SolidWorks now has a new feature available in sheet metal that will allow you to create “Rolled Edge Flanges”.  Its called “Swept Flange”.  With this new feature, you now have the ability to create complex sheet metal parts and create  flat patterns that go along with them.

Take a look at the example below...

Just like any sweep feature, you need to create both a profile and a path sketch (Note: with a sheet metal part, the path needs to be an open contour).  Once you have your sketches, simply utilize this new swept flange feature located in the sheet metal features...                                         

The results are just as you would expect...

However, as good as this new swept flange feature is, there is a slight problem when you go to show the flat pattern.  You will get an error stating that this part cannot be unbent...

Fortunately, there is a workaround.  The problem isn’t necessarily a problem with the geometry, but rather a problem with what SolidWorks thinks should be the fixed face/edge.  If you edit the flat pattern feature, you can clearly see what face SolidWorks is trying to keep fixed...

To get this flat pattern to work correctly, you will need to select an edge to remain fixed; Just as you would if this was a rolled cylinder without the flanges...

Once you tell SolidWorks what edge is to be fixed, the flat pattern will work as expected...

SolidWorks does have a handful of SPRs out there that address this very issue on similar parts as you see here in this example.  So if you run into a similar issue, look to see what SolidWorks is trying to keep fixed when flattening the part.  Most likely, this workaround will resolve the issue.

Even with the workaround, the addition of this new “Swept Flange” feature greatly enhances the sheet metal capabilities in SolidWorks.  You can now create more complex sheet metal parts than ever before.

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Custom Broken-out Section Views

Sometimes you may want to show a broken out section view in a drawing to see the inside of an assembly.  The broken-out section view tool that you have in the view layout tab can be difficult to control and doesn’t show well in an isometric orientation.  This can easily be done by creating an assembly feature cut.

I this case, I want to see the inside of the grill…

First create a sketch where you would like the cutout:

 

When you create the assembly cut, you have the ability pick and choose the components to be cut by using the feature scope.

 

Final results:

 

Now you can see the steaks cooking on the grill…

Enjoy,

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Finding the Center of Gravity in SolidWorks

As many of us know the center of gravity can be found easily in SolidWorks by going to Tools, Mass Properties. It shows a lovely pinkish purple triad in the place of the center of gravity. But shock when closing mass properties it goes away. But it's something that from time to time we need to stay visible.

I have found a macro that does locates a 3D Sketch point on the center but it is a one shot deal, move the mass around and the point is useless. But, there is another way.

There are SolidWorks variables in the equations pull down to use for center of gravity x,y,z. We just need to tie those to the point.

I have found a way to do this:
Use tools, equations to build three variables, type X=
then go to the bottom lower right hand corner and expand the drop down.
pick "SW-CenterofMassX" resulting equation should read X="SW-CenterofMassX"
Click ok, Repeat for y and z

insert a 3D sketch
create a point in the sketch
make sure the point is not on either the x y or z plane from the origin
dimension to the sketch point, use the tab key to convert the dimension from a point to point direct dimension to either an x, y, or z orthogonal dimension
right click dimension and use "Link Value" to attach it to the appropriate variable.

Notes on this use:
Make sure the model is mated so that there can't be any negative values for x,y,z positions of the center or mass. The mass will update a negative value but the SolidWorks dimension tool will convert it to a positive value, so it may end up with an improper location if the part/assembly is not in the positive half of the planes. For parts that you don't want to move off of the origin (for good reason), place the part into a new assembly file and place it in the positive area of x,y, and z.

Happy Modeling,
John Van Engen
CATI Tech Support

How to enter points with x, y and z coordinates?

Sometimes you may receive files from vendors or get information from a CCM where you need to plot out reference points using x, y and z coordinates.  There are not many tools in SolidWorks that will allow you to enter in x, y, z coordinates regardless of the feature type. 

One trick is using a 3D sketch…

In a 3D sketch:

1  -  Create however many points you need.  (Doesn't matter the location.)

2  -  Select a point.  Using the property manager on the left hand side, enter in the x, y, z coordinates of the point.

Note:  Parameters for any entity in the property manager are strictly for reference.  Entering values in the parameter boxes will NOT constrain the geometry.  Relations and dimensions are highly recommended to fully constrain sketch entities.

3  -  Because of the above note, the point is not constrained and is still floating in 3D space (hence the blue / under defined color).  This is one of the few times that it would be a good idea to use the “fix” relation so that you do not in advertently move the point.

4  -  Repeat the steps for the additional points.

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Swept Thin workaround.

A couple months ago I posted a blog on the differences between a solid sweep and a swept thin (http://blog.cati.com/2011/05/sweep-solid-vs-sweep-thin.html).

There is a work around to create a swept thin.  Surface sweep is the answer.

Note: For all these examples, the “pink” sketch will be used as the path, the “green” as the profile.

So, just as before, this is the shape we are after.

 
The sketches will be set up as so…

 

Instead of using a solid sweep feature, use a surface sweep .

Once you have the surface, use the thicken feature  to create a solid from it.

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

 

A Plethora of Plane Creation

How can you say I can create a Plethora of Planes if you do not know what a Plethora issss..

 
The other day in class I was reviewing plane creation when I heard, "I would say you have a plethora of planes." In a bad latin accent. That inspired a tangent that almost derailed the class.... Thanks Bill. But it got me thinking, "why not have a series on planes in the blog." So here it goes....

Chapter #1 - Plethora of Planes.

Would you like to create number of equally spaced planes in one shot. We you can in the plane creation command and its pretty easy. Start a plane, either from Insert, Reference Geometry,Plane or Control dragging on an existing plane in the view port. You will see this box.

 
By increasing this box you create multiple planes in one command at the same spacing. Take that Ned Nederlander.

Bob McGaughey, CSWE

CATI

Selection Manager

Surfacing Beginner,

You ever start a loft or a sweep and can't pick all the segments you need for a profile or guide. Well you should try the selection manager. It's found in the right mouse button click of the viewport when your in those type of commands. Here's example I did today.

 

As you can see it looks like the user was trying to loft 2 edges to a single edge. As you can see that didn't work. In comes the selection manager, which creates a selection group of multiple segments, edges, sketch geometry, that is treated as one element in the feature, awesome.... He cleared out the selection set and the right mouse button clicked in the viewport. Made his selections and hit the green check on the floating box to create that selection group. Stamp as DONE!!! as they used to say on Monster House.

 
 

Have great one, I'm off to do something... even if it's Wrong.

Bob McGaughey,CSWE

CATI

Mates and Flexible Sub-Assemblies (MSWP #10)

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).

Many SolidWorks users have never been shown the importance of mating methodology when working with large assemblies.  An Assemblies structure can make a significant difference in the performance of an assembly large or small.  These difference in performance is generally much more pronounced in a large assembly due to its shear size. 

The models that we used for our base line had a large number of top level mates and flexible sub-assemblies.  When SolidWorks brings up an assembly it has to solve all the mates that are at the top level.  This includes any mates at the sub-assembly level that are part of a flexible assembly at the top level.  The results of structuring the assembly to reduce the top level mates by creating more sub assemblies and turning off the flexible sub assemblies is impressive.

  
Results: 

• Opens 11% faster saving ~4 1/2 mins
• Rotations 34% faster saving ~ 10 1/2 mins
• Modeling 52% faster saving ~37 1/2 mins
• Closes 18% faster saving ~ 10 mins

As we continue through this series of articles I think you will find that modeling methodology and best practises far out strips hardware improvement for potential performance increases.  Having the best hardware possible does nothing for you if you don't use strong modeling techniques and use them consistently.

Adrian Fanjoy

Technical Services Director

Computer Aided Technology, Inc.