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.

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

Merging center marks

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

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

Add to center mark set

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.

  1. Start the Center Mark tool and choose Circular Center Mark.
  2. Select the two holes.  Orthographic center marks will initially appear in those holes.
  3. 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.
  4. Exit the Center Mark tool, then right-click on the center mark at the center of your part
  5. 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.

 

It may correct per the Standard, but it’s not pretty (until you see the alternatives)

An interesting thread appeared on the SolidWorks Forum this earlier this month. A SolidWorks user posted a question asking how to flip dimension text from one side of a dimension line to the other, for an ISO Standard drawing. The perceived problem was that a non-orthogonal linear dimension appears backwards to nearby orthogonal linear dimensions.

Should this Dimension be flipped?

Why would SolidWorks put dimension text on the wrong side of the dimension line? The user noted that if the dimension is placed on an opposite part (or other side view), the dimension text placement appears to be correct.

Dimension text seems correct here!

Actually, according to ISO standard, the 0.82 dimension is correct in both views! This is because the standard requires the dimension text to be in the most upright position. So, although vertically aligned text is required for vertical dimensions, dimension text should never actually be upside-down. This is a case where SolidWorks is following the rules of the standard, but the standard’s rules produce an affect that seems out of place to some users.

But are the alternatives actually better?

What would a flipped dimension look like in this case? What is really the expectation? As it turns out, this answer isn’t so simple, nor is it pretty. There is an ambiguity between two possible methods to flip this dimension.


Does this seem correct?
Although the 0.82 has the same reading direction as the 1.00 dimension, because 0.82 is nearly upside down, it is difficult to read.

Easier to read, but now it is oppose to other dimensions

This method is easier to read. But it still looks incorrect because it is actually oppose to other nearby dimensions. It also appears to be incorrect because now the dimension line is on top of the dimension text, which is more confusing (especially if you have a crowded drawing).

In general, this is a case where something may not appear correct at first, but once you see the alternatives, it really does make sense. These are the reasons why SolidWorks doesn’t support “flipped dimension text”. However, if you would like to use either of these alternatives, there is a workaround. Perhaps I will cover it in a future article.

What if you still want another solution?

There is one aesthetically pleasing alternative that SolidWorks and certain standards do support.

  1. Select Offset Text in PropertyManagerHighlight (select) the dimension.
  2. In the PropertyManager, select the Offset Text button.  The dimension text will now be attached to a leader that points to the center of the dimension line.  If this is fine, then you are done.
  3. For ISO Standard drawings, this may not be acceptable yet.  If this is the case, drag the leader so that it lines up with the dimension line, and the text is outside of the extension lines.  This requires a little bit of eyeballing, but nothing that is going to give you a headache.

Offset Text on a Dimension

Align leader of Offset Text to Dimension Line

New in SolidWorks 2014: Brief overview of Replace Model tool for Drawing Views

This entry is part 11 of 13 in the series New in SOLIDWORKS 2014

3DVision’s Super Sonic Ping Pong Balls

3DVision Technologies has created a Simulation study of a supersonic ping pong ball.  This is almost a how-to guide, including how to apply a Motion study to a static object.   Their disclaimer at the end is great, “Disclaimer:  No ping pong balls were destroyed as a result of writing this!”

Supersonic Ping Pong Balls

What’s New in SolidWorks 2013: Intersect (Wow!)

This entry is part 8 of 12 in the series New in SolidWorks 2013

SolidWorks 2013 introduces a new and powerful tool called Intersect. Intersect enables you to perform complex operations to quickly combine surfaces, planes and solid bodies in practically any way you need without the need for multiple cut, trim and fill features.  The tool’s visual interface allows you to do all the experimenting you’ll need in order to create the final shape you want.  The following is an example of how Intersect can help you to quickly build a part from multiple intersecting surfaces.

This is a set of surface bodies that will be used to create the exterior of a new consumer product.  The goal is quickly combine these surface bodies into a final solid shape that can then be shelled.

Series of surface bodies

  1. Intersect PropertyManagerStart the Intersect tool (found on the Features toolbar).
  2. Select all of the surface bodies.  As you select each one, they populate the Selections box in the PropertyManager.  Hint: you can use window select to get all the surface bodies at once.
  3. Choose Intersect button.
  4. A list of intersection regions is quickly generated in the Regions to Exclude box in the PropertyManager.  In the case of this project, there is only one region, so there will be nothing to exclude.
  5. Make sure Merge result is checked on the Options box in the PropertyManager.
  6. Because we do not want the surface bodies to remain in the final part, make sure Consume surfaces is also checked.
  7. Once you are satisfied with the previewed result, choose OK (green check mark button) to accept and apply.
  8. The result is finalized.  The entire operation appears as one new Intersect feature in the Feature Tree.
  9. Adjustments to your selections can be made at any time by editing the Intersect feature in the same manner as any other features are edited.

Preview of result

Preview of result
Final result
 Final result

Pointy arrows without the ears (a.k.a, text)?

Every once in awhile in drafting, you just need an arrow, with no text, attachments or any other extras.  Maybe you need to specify air flow, grain direction, inspection queue, assembly instructions, or one of a hundred other reasons.  How do you make just an arrow in SolidWorks?  Answer: Multi-jog Leader annotation tool.

Mutli-jog Leader is an oft overlooked tool that pretty much lets you make whatever arrow configuration you like using the same leader style of notes. 

To make a simple leader with no text, start the Multi-jog Leader and select your first point.  One arrow will point to the location where you clicked.  The other end of the leader will follow the mouse cursor.  Choose a second location and double-click to complete your leader.  This will add another arrow directly opposite your first arrow.

Get rid of one of the arrows by RMB clicking on the tip of the undesired arrow and choosing the arrowless option.

 

Here’s what you end up with. 

You can adjust the other end to be bigger (by RMB clicking on it and selecting Size…). In the case of the example below, I’m using the arrow to represent fluid direction of a flow body.