SW2012 Equation Manager - #1 In My Book!

As I begin to dig deeper into the 20th release of SolidWorks, I am finding that the little enhancements seem to impact me as a user much more than any of "Major Enhancements".  Whether is it storing blank Custom Properties or not inserting a hole when launching the Hole Wizard, the little "tweaks" to existing functionality are the ones that make me smerk.

Equations, which by the way were ear-marked with the "Top Enhancement" orange star ,ended up being my personal favorite ehnacement to SolidWorks 2012 since building intelligence into models is something I do a lot.  SolidWorks 2011 started this trend with the addition of Global Equations and control of suppression states with the VB's IIF statement.  As the functionality has grown, there are far too many features for the current interface, especially for those of us that began adding a bunch of automation to our files.

SolidWorks 2012 has completely overhauled the interface, adding a number or organizational control such as filters, views and pre-populated lists in addition to new functionality.  Here are a the various view options with a few things pointed out:

                                             

On the functionality side, the new Equation Manager can determine the solve order to avoid those blasted "CIRCULAR REFERENCE" issues we get when tying ourselves in equation knots.  This reminds me of SWIFT (SolidWorks Intelligent Feature Technology), where the tool attempts to determine the best route to solve the issue for you.  Although this is not going to fix all your problems ("That was easy") but it might take some troubleshooting time out of the equation ;-).

Here are a few of my favorite additions, although I like them all, especially the new UI!: 

1 - Measure Option:

This new addition basically allows you to create on the fly criteria for evaluating your equations.  By using this new option, a distance on the active model can be used without having to pre-add a reference dimension in the model, making the process of adding automation fast.

2 - Browse and Open buttons linked external equation files.

Last year the abiliy to link files was very interesting to me, however it was not straight forward how to link and easily edit these files.  In 2012, checking "Link to external file", you are prompted with this message to use an existing file or create a new one.  Once linked it is simple to select a different file and also easy to edit the linked file.  By clicking on the Open icon, Notepad will lauch with the linked file loaded, allowing quick editing access. If you decide to add new columns, you can just reimport it, which will add the missing rows in the Equation interface.

This is a huge improvement to linked files and has lowered the barrior of entry for new users to take advantage of this cool feature.

3 - Automatic Rebuild:

This last pic might seem little but the ability to rebuild the list of equations as you make changes in the Equation editor is very convenient.  There is also a rebuild button located to the immediate right that will rebuild the file on demand.  This is especially handy if you make modifications to a linked file and want to see the values update in the Equation manager.

The What's New PDF outlines this revamp of Equations very well and provides a few examples to show all the new additions.  I recommend trying this new feature out when you get SolidWorks 2012 installed! ~Lou

SolidWorks Auto-space For Linear Patterns?

Circular patterns, on most platforms, have the ability to equally space when adding patterns around an axis but what about linear patterns?  Linear patterns in SolidWorks have some very powerful tools to vary the sketch and omit instances but lack the check-box option "Equal spacing".

A few releases back, SolidWorks introduced the Fill Pattern tool that populates an open field with a feature, giving options to control various spacing criteria.  Although useful for creating cutouts for venting, the tool does not address patterns along an edge or situations where the fill needs to equally spaced or split on the border, as pictured to the left.

Solution: Curve Driven Patterns!  Who says a curve can't be a straight line, well in SolidWorks at least? This option will allow an edge to be selected and, similar to it's Linear counterpart, enter the spacing increment in addition, have the option to select an edge and check "Equal spacing".  Now as the size of the model changes, the pattern will maintain the population count but keep the spacing equal without having to manually adjust the increment or write an equation to control it.

I used this approach for a local customer trying to automate a grate design and having the requirement of the cutout to be not only equally spaced but bisected along the edge for aesthetic reasons.  It was then automated using DriveWorksXpress and rules were written in order to control the number of instances based on the size without requiring multiple rebuilds using equations in SolidWorks. ~Lou

Automatically Vary A Pattern

For an old feature, vary sketch still gets a lot of praise from those that use it. It can be very useful when wanting to use a linear pattern but need to have some adjustment happen on some of the instances. The picture to the left shows what happens when you take a seed (thru cut on the far left) and propagate it without the vary sketch option using a linear pattern along the bottom edge. Vary sketch can adjust the cut but it requires some design intent in the sketch geometry to work properly.

When you create the sketch for the feature you are going to pattern, you need to make sure that the sketch has a feature that will adjust as it patterns. For example, the top part seed feature is an offset of the spline shape of the top of the part. This allows the top of the part to adjust as the feature's horizontal locating dimension is changed.

The trick to using the vary skech option is that instead of selecting the bottom edge of the part as the direction vector, you would select the locating dimension of the seed feature. In the example picture, the locating dimension to use would be the dimension that locates the leftmost side of the seed feature to the left most edge of the part. Once you select this you will see the preview of the linear pattern as you would if you selected the bottom edge. Now check the vary sketch option. You will notice that the preview will dissappear and I believe this is a bug, which I have submitted but has never been fixed! Anyway, when you click on OK you will notice the following result (picture to the right). This option tells SolidWorks to pattern using the locating dimension as a driver to change the sketch as it would by changing the dimension. If you haven't seen this feature before it can be an eye opener! ~Lou

Extruding A 3D Sketch

This is a followup post to episode 92 when I discussed 3D sketches in SolidWorks. As I mentioned, many people don't realize that you can extrude or cut with a 3D sketch as long as it is closed and it has a vector direction to extrude along. As you can see, selecting the 3D sketch will be a contour that creates a fill surface and your direction can use a linear edge or sketch. It will essentially perform a directional sweep but this direction option can be useful for 2D sketches as well, in the event you don't want to extrude or cut normal to the sketch plane.

I also mentioned that you could use this to cut a free form directional cut into a complex surface using the spline on surface command. This command can be found under Tools, Sketch Entities, Spline on Surface. Once launched, the command will begin a 3D sketch and allow sketching on a complex surface, which will automatically reference the spline points coincident with that surface. Once finished, sketch a straight line in the vector direction of the cut, which could be within the same 3D sketch, or select a linear edge of the part. Now launch the Cut Extrude tool and select the straight line as the direction component and select the spline on surface as the cut contour.

This is one of those features that may come in handy for those obscure applications so I thought I would add a visual aid to follow the podcast. By the way, in case you were curious, this was added back in SolidWorks 2004. ~Lou