Graphics Systems SolidNotes

Click, Snap! Using Named Mate References with Sub-Assemblies

If you're like me, you want to save time.  You want to be more productive. And SolidWorks has many tools to aid you.  For example, creating the needed geometrical relations between components in an assembly (called "mates") is sped up with SolidWorks' "Smart Mates" technology.  Hold down the ALT-key, click and drag a face or an edge over to other geometry.  Viola!  A new mate (or two) is quickly created.

In the same vein, mates can be pre-described on components such that they more quickly snap in to place when inserted in to an assembly.  These are called "Mate References."  AND, if the Mate References in the part has the same name as a Mate Reference in the assembly then you can save even more time! However, the terminology in SolidWorks' Help file refers specifically to the use of Mate References with regards to individual parts (components) only. Does this mean you can't do the same with sub-assemblies?

Thankfully the answer is a resounding No!  With a little extra reference geometry, one can easily leverage Mate References for sub-assemblies to allow them, also, to SNAP in to place in a top-level assembly.  I'll show you how:

I begin with creating common reference geometry in both the sub-assembly and the top-level assembly.  In the images to the right, you see just that.  (you do not have to name the reference geometry identically but it helps from a documentation standpoint)

You then create an identically named Mate Reference in both the sub-assembly and top-level assembly.   Select the appropriate reference geometry items to populate the Mate Reference in addition to their appropriate mate conditions and alignment. (see the thumbnailed image to the right)

The thumbnailed images below show the two identical Mate References I added to both models. When the sub-assembly is inserted in to the top-level assembly, you need only click once to finish placing it. See the image below.

And the final assembly tree, complete with mates, you can review by clicking the last thumbnailed image to the right. You can see, hopefully, that with the right references in place, using named Mate References will allow you to quickly insert your sub-assemblies in to upper-level assemblies.

Flattening a swept helical part

In the case of having to model a sheetmetal "rail" with a helical profile, one is left- oftentimes- trying to model a cylinder, unfold it, and cut away excess material only to find that it fails to re-fold correctly. However, there is a suitable case where a user can model a helical sweep, insert bends, and unfold it for the purposes of adding features. But let us first look at what defines a helix as well as a sheetmetal part.

The helix functionality of SolidWorks is an inserted Curve and is created from a simple, planar sketch of a circle. The options to create and control the helix include:

1. Pitch and Revolution- the number of revolutions by the over-all pitch of the curve
2. Height and Revolution- the over-all height and number of total revolutions of the curve
3. Height and Pitch- the over-all height and total pitch of the curve and
4. Spiral- a 2-D/planar spiral controlled by the total number of revolutions.

The outer diameter is controlled with the intial sketched circle. The pitch is defined as the total linear travel divded by the number of revolutions. So, for example, a height of 4in and pitch of 8in would result in 1/2 of a turn (180 degrees of revolution).

And this is paramount because, in order to flatten a helical swept feature, the pitch can not be less than 1/2 the over-all height of the curve and can only be whole, constant value multipliers. Or, in other words, in a curve with a height of 4in and a pitch of 8, the pitch may be set to multiples of 2x, 4x, etc. This, however, will allow SolidWorks' sheetmetal functionality, Insert Bends, to create a valid sheetmetal part that may be unfolded to the flat pattern.

When a non-sheetmetal part has bends inserted, assuming SolidWorks can unfold it, two types of bends are created: Flatten and Process. The Flatten Bends do just that: they flatten the part. In the case of a cylindrical or a helically swept part, the Flatten Bend type is a round bend.

A sheetmetal part is also defined by or controlled with what is called the "k-factor." This value differs by material type, gage,  and processing. But, to simplify the definition the k-factor is the neutral acis situated within a bend. There are excellent resources on-line at both www.sheetmetaldesign.com and www.sheetmetalguy.com; I'd encourage you to visit those sites.

Lastly, in order to create our helical part, we need to sweep a closed profile that is designed to the thickness of our material. This profile is swept about the helical curve we created.  Sheetmetal bends can be inserted after the sweep creation and additional cuts can be added after folding and re-folding. Click here to download an example file.

Min/Max Your Dimensions

SolidWorks has three different attachment points when dimensioning a distance to and arc or circle. The arc conditions are described below.

Center: The default when an arc is selected. Dimension attached to the center point of the arc.

Minimum Distance: Attachment point is to the closest point on the arc on the same die of the center as the other end of the dimension. Linear dimension does not cross arc centerpoint.

 

Maximum Distance: Attachment point is to the farthest point on the arc on the opposite side as the other end of the dimension. Linear dimension crosses arc centerpoint.

Selecting an arc as part of a linear dimension causes the dimension to default to the center arc condition. However, if the Shift key is held down as he arc is selected for a linear dimension, the arc condition will be minimum or maximum, whichever is closest to the side being selected.

Further, the arc conditions) of a dimension can be changed after the dimensions is created. Right-click on the dimension, select Properties, and  change the arc condition by selecting the new option near the bottom of the dialog box.

Note that there can be two arc conditions to control if the linear dimension is between two arcs.

Modeling a knurl in SolidWorks

Sometimes a creative solutiuon will solve a problem when there isn't a "do this" button. One request I've received over the years is to find a way to show a knurled surface on a model. This is how I do it:

1. Create a sketch of one facet of the knurl. For example, a diamond. Position it on a plane hovering over the surface you want, such that the sketch is on one edge (top edge of a cylinder, etc.)

2. Use Wrap feature to wrap the sketch onto the model. Use the "scribe" option in the Wrap command so that it will simply break out a seperate surface showing the facet.

3. Use the Offset Surface command to offset a surface body of the facet. You'll need to offset a certain, but tiny, amount in order for the hidden lines to show up clearly all on the drawing views when doing Step 4. I typically use .005" when I do this.

4. Use the Pattern command to pattern the surface body as needed to cover the model area.

That's it! You'll see the facets in the 3D model and they should also show up nicely in the 2D drawing. If they "fade out" in the views near the tangent edges, then you need to increase your offset a bit. Again, I find that .005" is enough whenever I do this on my models. This method is also relatively low on system overhead and it's very easy to suppress the knurling as desired.

You can download an example model at http://www.gxsc.com/SolidNotes/knurl_example.zip