Many of us have been arms wide open to the new section view assist tool that was released with SolidWorks 2013 but for those who have yet to make the move, this blog is for you.  I have seen it a few times now, a customer calls in and is finding that their jogged section view is stretched when this is not the view they intended.  Generally, the option for creating a “foreshortened section view” or “an aligned section view” comes up when selecting a jogged section line for creation of the section view.  This message can and is often times dismissed leaving the user to default to the last selection.  One option is to clear this message from the System Options under messages/errors/warnings; the second option is the topic of this blog.

 

Let’s take a look at an example of a created section view, I have sketched in my line, inferenced my geometry and selected the section view.  I was prompted the above notice in which I wanted to create an aligned section view for purposes of this post.

The section view was created and as you can see an aligned section view was generated from my selected sketch line.

Now this may not be the desired section view, so how can I go about creating a foreshortened section view where the projection is normal to the cutting line?  Simple!  If you go back to the option of the two, you will see in the description that “Construction lines are excluded from the view.”

I can simply edit the sketched line that I used to create the initial aligned view, but change the vertical sketched line to construction lines.

After this has been done, simply exit the sketch and your section view will update to a foreshortened section view.

Pierce and coincident, aren’t they the same thing?

They are the same in that they are both sketch relationships, but that’s about as far as that goes.

SolidWorks defines a Pierce Relation as a relation that makes a sketch point coincident to the location at which an axis, edge, line, or spline pierces the sketch plane.

Okay…so what does that mean?

Let’s take a look.

I’ve created a spline on my top plane and a circle on my front plane.  If I choose to make the circle and the spline coincident the center of the circle will move on the sketch plane to be coincident with the spline but not touch the spline.

Let’s look at this from a few different angles.

From a view normal to the sketch plane we can see the coincident relationship.

I can move the circle on the sketch plane and it continues to maintain a coincident relationship to the spline.

But if we look from a different angle (let’s say the top), we see a much different picture.  The circle may be coincident with the spline when looking at the sketch plane, but it doesn’t actually touch the spline.  The spline does not pierce the circle at any point.

However, when I add a pierce relationship, which is a 3-dimensional relationship, the circle is now moved to a location where the spline pierces or passes through the Front plane, our sketch plane.

Neat, huh?

Okay, but if we look at our spline we can see it pierces or passes through our sketch plane at a number of places.  How do we select the exact location where we want our circle to have a pierce relationship?

It’s easier than you may think –

By selecting the spline closest to where it passes through the sketch plane, the circle will move to a place where the spline pierces closest to that location.

Super neat, huh?

Okay, so why does all this matter?

Well having a pierce relationship is nearly critical when creating a sweep.  Here’s rule of thumb, when you create a sweep, create your path first and your profile second.  If you create them in the opposite order you will not be able to create a pierce relationship between the two sketches.

Take a look below.  I’ve created a profile, a path, and two guide curves.  I’ve set up my profile using coincident relationships with the path and guide curves.  Notice the profile also has vertical and horizontal relations.

Whoa!  Not good folks, not good.  Let’s see if we can fix this a bit and get better results.

Using the same set of sketches, I’ve updated the relationships on the vertices of the profile to pierce the path and guide curves.  I also changed the horizontal and vertical relations to perpendicular and parallel.

Why did I do this?  Look at the result, much better.  Phew!

By using relations that don’t restrict the profile (horizontal and vertical are restrictive) it allows the profile to rotate independently along the sweep.  By using a pierce relationship at the vertices, it also allows the profile to move along the path and maintain a pierce relationship yielding a much better result.

Pierce and Coincident, the same thing?   They are the same as much as apples and oranges are the same.  They may both be fruit but that’s where the similarities end.

 

 

 

 

 

SolidWorks 2013 is finally here and it’s loaded with great enhancements, including those that will help with the overall performance of such powerful software.   One of these features is a great addition to the already existing “Assembly Visualization” tool that you can find in the evaluate command manager within an assembly.  Before, you were able to sort and view your assembly by custom properties,  now 2013 allows you to take a look at your assembly by Graphics-Triangles, which creates a tool to analyze why you might have slow performance within an assembly due to a complex geometry.

Once you have your assembly open, click the Evaluate Tab and find the Assembly Visualization Tool, or from the Tools drop down> Assembly Visualization.

 

From here you have the option to define an array of columns with different definitions: filename, mass and quantity are created by default.  Click the arrow directly to the right of mass to create your own column by choosing either to add a new column or redefine the mass column.    Since we are trying to review the assembly by complexity of geometry within parts, click ‘more’ and from the properties menu select ‘Graphics-Triangle.’

 

 

 

You can now sort the columns by clicking on the title of the desired column to sort; for this example, click on the Graphics-Triangles to sort from highest to lowest.  Now you are able to select the parts that have the most complex geometry to simplify, review or whatever might meet your needs.

 

 

To learn more about what’s new for 2013, reserve your first look!!

http://symsolutions.com/SolidWorks-2013-Launch-Events.html

 

Text wrapping is a fairly simple tool to use within Solidworks part modeling when you are applying a wrap to a flat face or around a cylinder, but when you run into a part with a changing radius and a rounded face, the wrap feature becomes a little more complex.  For this example, we will wrap text onto a conical feature.

In order to create  this text wrap, we must first create some construction geometry that is relative to the dimensions of the cone.  By identifying the point where the axis of the cone and the plane of the cone intersect, we can use this point to further create a half circle on our sketch plane.  So lets go ahead and define this point.

 

Now create a plane tangent to the face of the cylinder; this plane will be used to add the text and text curvature.  You will see that the distance of where the text is placed is going to be the radius of the half circle we create in the next step.  In this example, the text is located 4.7 inches down from the top of the conical section, so go ahead and create a half circle arc with a radius equal to the distance you want the text to be relative to the tip of the cone.

Now all of our construction lines are in place, insert the sketched text and click the arc to create the correct geometry for the text to be wrapped.  Make sure that the text inserted is on the same plane you created but inserted as a different sketch than the construction lines you have created.

 

Click the wrap feature, choose the sketch of the text you are wrapping and the face of the cylinder and you are all done!

I have always found that the routing tools to be an interesting part of SolidWorks but was never able to really learn all the ins and outs of it. So a while back I started looking a little closer at it. I am right now working from the Piping & Tubing portion of the training manuals.

I always thought the rules for creating the routes were very consistent and that you needed to have connector points (CPoints) and route points (RPoints) to be able create any route. Well I found a tool to be able to start a route without a connector.

This is very helpful if the component you are using is an imported model from a vendor and they supply the connector but you are not sure what it will be. They did let you know the size of pipe/tube/wire and a location for where it will be on the component. So know if it is not all ready on the model you will need to create a cylindrical cut to represent the start point.

 

The tool to use in this instance is Start at Point and is available on the all three routing tool bars Electrical, Piping, and Tubing. Once you select the appropriate tool you then select the cylindrical face from the hole for the starting point and it gives you a nub start so you can then continue the route in whatever manner you need to complete this.

So as I continue to dive into the routing tools I will add any interesting features that may be hidden or not really well known.