SOLIDWORKS X-ray Vision with transparency

SOLIDWORKS that allows you to quickly view your entire model as transparent mode, like an X-ray of your assembly.

Top Level Transparency is an option within SOLIDWORKS that allows you to quickly view your entire model in a transparent mode. It’s like a quick-access x-ray of your model. You may need this to peer deep into the heart of your assembly. Perhaps you are trying to visually find an obscured part which is buried within your assembly. Even within an individual part, you may just want to see a particular set of features without a section view.

You don’t have to change the transparency of each and every component within your assembly or create special display state. Just turn this setting on, and then turn if off.

How to turn Top Level Transparency on

To turn it on, right mouse button click on the top line of your Feature Tree. Select the Top Level Transparency option from the shortcut bar or within the list of options of the right mouse button menu. Repeat to turn the mode off.

Although Top Level Transparency is a mode, it does directly affect the transparency of the assembly and components while active. This means the setting is persistent. If you turn this setting on for a component, when you open the associated assembly, that component will be transparent within the assembly. A component or assembly can also be saved with this mode active.

Besides Transparency, explore changes to Exploded Views

Another assembly tool that you may wish to explore in SOLIDWORKS might be Exploded View, which has seen a number of enhancements over the years. SOLIDWORKS 2015 introduced Radial Explode. Back in SOLIDWORKS 2013, you gained the ability to copy exploded views. More recently, you have the ability to autospace exploded components.

Each release of SOLIDOWORKS sees many enhancements for assemblies. Be sure to always review each year’s What’s New document.

Return of Ctopher’s Custom Material Database

ctopher custom materials for SOLIDWORKSCustom materials in SOLIDWORKS are important if you are using materials not included in the default set.  Around a decade ago, Chris Saller compiled a bunch of such custom materials from varies sources based on requests and submissions from many different people.  This list is informally known as Ctopher’s Custom Material Database, “ctopher” being Chris’ handle.

Various versions of this file have been available on now long-gone websites over the years.  Well, the material database is finally back and bigger (better) than ever!  Chris has complied a new version in SOLIDWORKS 2016.  This new version has many new materials.  The new database is now available directly on SolidWorks Legion in the File Downloads tab as Ctopher’s Custom Material Database.

There are two methods to point SOLIDWORKS to use a custom material database.  The easiest method is described on Ctopher’s Custom Material Database download page.  Below is a slightly more advanced method which should also work on networks.

To point SOLIDWORKS to make the materials in this database available:

1.To use, place custom_matls_091516_sw2016.sldmat file into an easily accessible folder, such as S:\SOLIDWORKS Shared File\Custom Materials.  The folder is your choice, based on your network and operational set up.


3.Goto Tools>Options…>System Options>File Locations.  In the Show folders for dropdown, select Material Databases.

4.Select Add button.  Navigate to your chosen folder, such as S:\SOLIDWORKS Shared File\Custom Materials.

5.Select OK button.

6.Repeat for all instances of SOLIDWORKS within the network that need to access this database.

To use the custom materials:

1.Open any part file.

2.In the Feature Tree, right click on Materials and then select Edit Materials.  “Custom_matls_091516” folder will be on your material list.

4.Click on desired subfolder, such as Copper Alloys.

5.Click on desired material to view properties.

6.Click on Apply to apply that material to your part.

7.Click on Close to return to your part.

Ctopher’s Custom Material Database

Not seeing sharp corners when using thick lines?

Thick line corner gapHave you ever noticed there is a gap on the corners of your lines when you have model edges or sketch lines?  You will usually notice this when you try to use very thick lines on a SOLIDWORKS drawing.  Why are you seeing this gap?  Welp, as with most visual display characteristics in SOLIDWORKS, there is a setting for that.  You actually have three options for corner appearance: Flat (default), Square and Round.  This is found in your drawing’s document properties at Tools pulldown>Options…>Document Properties>Line Font on a setting called End cap style.

End cap style


Flat is the default option and normally works fine for most cases.  However, if you are using much thicker lines, you can utilize one of the other two options to get the look you need.  It is important to note that this setting applies individually to each of type of edges, so you can use a different end cap style for sketches than you use for visual edges.


Square end cap style


Round end cap style

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

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


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.


Copying sheets from one drawing to another

It’s been well over a year since I’ve done a raw tips and tricks posting.  That’s a year too long.  So, here’s a quickie!

In SOLIDWORKS drawings, you can copy a drawing sheet from one open drawing to another open drawing via the right-click menu in the Drawing Tree.

  1. Open the copy-from and copy-to drawings.  Make the copy-from drawing active.
  2. 6-5-2014 12-38-07 PMIn the Drawing Tree, right-click on the drawing sheet you wish to copy.  The right-click menu pops up.
  3. Choose Copy from the menu.
  4. Activate the copy-to drawing.
  5. Right-click on the drawing sheet that is near the position where you wish to add your copied sheet.  The right-click menu pops up.
  6. Choose Paste from the menu.
  7. A dialog will pop up asking if you wish to insert the new drawing sheet below or above the selected sheet, or if you wish to add it to the end.  Make your selection and choose OK.  The copied sheet will appear at the specified position in the Drawing Tree of your copy-to drawing.


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