SolidWorks Legion

Adding your ideas to SOLIDWORKS World 2015 Top Ten list is easy

SOLIDWORKS World 2015 in Phoenix, AZ is just over 100 days away. A tradition of SOLIDWORKS World is the Top Ten list, inwhich customers submit their ideas on how SOLIDWORKS can be improved for them, and then vote for their favorites. The top ten vote getters are announced on the mainstage at SOLIDWORKS World. It’s easy to submit ideas. You don’t have to be attending SOLIDWORKS World to submit or vote. Input from all customes is welcome. Here’s a short video.

If you have an idea, here’s somethings you can do to improve the attention your ideas gets:

Your idea’s title should be a complete thought. For example, “Ability to change colors for sketch lines on-the-fly” is much better than “Change colors”.
Your idea’s description can be as long or as short as you need.
You can add images to illustrate your ideas.
Break out separate ideas into separate submissions, even if they are related. For example, you may have several ideas on how to improve Weld Symbols, such as improving the interface, adding new symbols, and adding new controls. Although those these are all regarding the same tool, they are really three different ideas, each of which deserves to be voted upon separately by everyone.
Quickly respond to comments posted by others on your ideas.

I also recommend commenting on other ideas you like, dislike or feel needs more clarificaiton.

Have fun with your submissions at SWW15 Top Ten List (don’t forget you’ll have to sign in to the SOLIDWORKS Forums before you can submit). And when the polls open, vote early and vote often (on as many ideas as you wish).

Year of the Angle Dimension (Part 4): Symmetricality

This entry is part 4 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

Previous releases of SOLIDWORKS introduced linear dimensions in sketches that can be applied symmetrically when created across a centerline. Further enhancements saw smarter behavior, where the selected centerline is remembered for multiple dimensions created in sequence. For SOLIDWORKS 2015, you can create multiple half and full symmetric angular dimensions without selecting the centerline each time.

To create a symmetrical angle dimension:

In a sketch with a centerline and lines or points, click Smart Dimension at Tools>Dimensions>Smart.
Select the centerline and another line which is at an angle to that centerline.
To create a half angle dimension, move the mouse cursor to the desired location and click to place, as previously. However, to create a full angle dimension (across the centerline), hold down the SHIFT key.
Drag the mouse cursor (along with the previewed dimension) to the opposite side of the centerline. As you do so, a preview of the angle dimension will appear symmetrically about the centerline.
Click to place dimension as desired.
Keep holding down the SHIFT key and select other lines at angles to the centerline. Angle dimensions to the centerline will automatically generate and will allow you make more symmetric angle dimensions successively.

Year of the Angle Dimension – Part 3 – Goodbye Zero

This entry is part [part not set] of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

When you use angles that are set to deg/min and deg/min/sec, there are often times when you’ll have zero (0) for one of the levels of units. For example, an angle may be 43 degrees, 0 minutes and 20 seconds. This is displayed as 43° 0′ 20″. For many people, the 0 minutes is redundent and unnecessary. SOLIDWORKS 2015 now has an option that allows you to show only the unit levels that have a non-zero value. For this example, the display is 43° 20″. This new setting can found at Tools>Options>Document Properties>Dimensions/Angle, and named “Remove units with 0 value for deg/min and deg/min/sec”.

Year of the Angle Dimension – Part 2 – Flipping out (and over)

This entry is part 2 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

In SOLIDWORKS 2015, there are two methods to change (flip) an angle dimension.

Vertically Opposite Angle

You can now flip any placed angle dimension to its vertically opposite angle. This is useful when you wish to place the entire angle dimension outside of the model edges.

Right-click on the angle to bring up the right-click menu.
Select Display Options, then Vertically Opposite Angle.

Explementary Angle

You can now flip any placed angle dimension to its explementary angle. Here is a way overly complex video about explementary angles. Here’s a simpler explanation straight from the dictionary.

Right-click on the angle to bring up the right-click menu.
Select Display Options, then Explementary Angle.

Choose Explementary or Vertically Opposite in dimension preview

When creating an angle dimension with Smart Dimension tool, you can now choose between the explementary angle or the vertically opposite angle during the preview by holding down the ALT key when the mouse is in the vertically opposite region. In SOLIDWORKS 2014 and prior, you were only offered the explementary angle.

Year of the Angle Dimension – Part 1 – Imaginary Rays

This entry is part 1 of 5 in the series SOLIDWORKS 2015 - Year of the Angle Dimension

There was a heavy focus on expanding functionality of angle dimensions using the Smart Dimension tool in SOLIDWORKS 2015. These enhancements streamline drawing detailing and sketch creation tasks. Here’s the first of such enhancements.

There is a long standing request for the ability to apply angle dimensions where one ray is aligned to geometry (model edge or sketch line) and the other ray is along an imaginary vertical or horizontal direction. In SOLIDWORKS 2015, there is a new capability with Smart Dimension tool that enables you to create this type of angle dimension.

Start the Smart Dimension tool.
In a drawing view, select a model edge.
Select a collinear and adjacent point (vertex or sketch point).
A crosshair appears over the selected point. Select one of the crosshair’s segments.
A preview of the angle dimension appears.
Click to place the dimension.

Apply your Center Mark and actually using it too (with advanced right-click commands)!

This entry is part 2 of 9 in the series New in SOLIDWORKS 2015

For what do we use center marks? Center marks are a drawing standard annotation placed at the center of holes and other radial features. This allows a drawing reader to see two things quickly. First, they can immediately see the feature is radial (hole or fillet). Second, they can quickly identify the center of that feature. Dimensions placed on hole typically originate from the hole’s center, where the center mark is placed. This adds clarity to the drawing.

Holes with and without center mark

Center mark applied to the right hole

SOLIDWORKS Center Marks

It seems like every year, there’s one or more enhancements for center marks in SOLIDWORKS. In SOLIDWORKS 2009, center marks for slots was added. SOLIDWORKS 2010 saw smarter center marks, which applied the appropriate gap from the dimension’s extension line, even if the center mark was placed after the dimension. SOLIDWORKS 2011 and 2012 saw the added abilities to automatically apply center marks in more situations. Center marks could be automatically applied to a default layer in SOLIDWORKS 2013. In SOLIDWORKS 2014, center marks can be added to Hole Wizard slots. And, SOLIDWORKS 2015 now includes the ability to add center marks to a set of center marks, reattaching dangling center marks, and automatically applying connection lines to center mark sets upon creation. This is just the past five releases. Center mark enhancements have been added nearly every year since Drawings was first introduced in SOLIDWORKS.

SOLIDWORKS has many center mark capabilities in Drawings. The c0llection of What’s New items listed above form only a short list. Here’s some tips and tricks you may not know about.

Center Mark tool creates three types of center marks

When you start the Center Mark tool, a PropertyManager comes up that allows you to set properties for the center marks you are about to create. In the Manual Insert Options group box (about the middle of the PropertyManager), there are three buttons: Single Center Mark, Linear Center Mark and Circular Center Mark. Single Center Mark (top left) makes individual center marks that aren’t associated with other. Linear Center Mark (top center) creates a set of center marks in a linear (x,y) pattern. Circular Center Mark (top right) creates center marks in a circle pattern. With Linear Center Mark and Circlar Center Mark, a set of center marks are created, allowing you to apply connector lines between center marks for clarity.

Linear Center Mark requires two selections to form a set (two holes).
Circular Center Mark requires three selections (three holes) so that the center of the pattern of three holes (presumably on a bolt circle) can be established.

Manual Insert Options

Adding new center marks to an existing set of center marks

As of SOLIDWORKS 2015, there are now two methods to add center marks to a set of center marks (Linear Center Mark or Circular Center Mark).

The first method existed before SOLIDWORKS 2015. It involves merging one existing center mark with one existing center mark set.

Select any portion of the center mark set.
Hold down the CTRL key and select an independent center mark.
Right-click on either the set or the independent center mark, then release the CTRL key.
In the right-click menu, select Merge Center Mark.

The second method is now available in SOLIDWORKS 2015. This new method doesn’t require an existing independent center mark.

Right-click on any portion of the center mark set.
In the right-click menu, select Add to center mark set.
Select every hole to which you wish to apply a center mark.

Delete individual center marks

To delete a center mark from a center mark set, simply select the center mark and strike the DELETE key. The center mark set adjusts automatically.

Delete a whole center mark set at once

Double-click any portion of the center mark set. This will select the whole set instead of just one element. Strike the DELETE key. The entire center mark set will be deleted at once.

Reattach dangling center mark

In SOLIDWORKS 2015, you can now reattach a dangling center mark. (A dangle center mark is one that is no longer attached to its original geometry.) Simply right-click on the dangling center mark and select Reattach. You can then select a new hole to which the center mark will be attached.

Advanced tip for Circular Center Mark

If you have a bolt circle of only two holes on a round part, you might experience a limitation of Circular Center Mark. As mentioned above, you need three holes to create a center mark set with Circular Center Mark. You can also create a center mark set using just two holes and exterior geometry. However, if exterior geometry is not available, there’s just an extra couple of steps.

Start the Center Mark tool and choose Circular Center Mark.
Select the two holes. Orthographic center marks will initially appear in those holes.
Select the outer geometry of your round part also. This will put the center of the center mark set in a strange location, but that’s ok.
Exit the Center Mark tool, then right-click on the center mark at the center of your part
In the right-click menu, select Set Base Center. This will now make the center of your bolt circle to be the center of the part.