Automatic Border tool works its wonders

Check out SOLIDWORKS’s Automatic Border tool and how it makes editing your Sheet Formats so much easier than old fashioned sketching!

SOLIDWORKS has the amazing Automatic Border tool for Sheet Formats. You don’t need to sketch your drawing borders from scratch. You also do not need to edit many sketch objects to update your borders.

The Automatic Border tool allows you to control all elements of your drawing border and associate those with drawing zones which are intrinsic to the drawing sheet. The tool has many functions to provide to you the ability to make and edit your borders to your exact needs.

To support ease of editing your Sheet Formats, a tab is available on the CommandManager called Sheet Format. This tab includes the tools Edit Sheet Format, Title Block Fields and Automatic Border. To find the Automatic Border tool:

Click on the Sheet Format tab
Choose Edit Sheet Format to switch to Sheet Format mode. Then, select Automatic Border tool.

On a newer template created in SOLIDWORKS 2016 or later, your border will highlight as orange. (If you have an older Sheet Format or you are trying to incorporate your old Sheet Format from another CAD application, see SOLIDWORKS Help.) In the Automatic Border PropertyManager, select Next to edit your existing border.

The first page of the PropertyManager is for legacy (pre-SOLIDWORKS 2016) Sheet Formats. If you have a newer Sheet Format, just skip this first page by selecting Next.

On page two of the Automatic Border PropertyManager, you have many options to edit your border.

Zone size and Margins

Zone Size groupbox allows you to establish your zone distribution and region.

The 50mm from center option under Distribution allows you to use a common size and placement regardless to sheet size.

Evenly sized option allows you to automatically divide the sheet up into evenly sized zones, including a custom number of rows and columns.

Under Regions, you can set zones to fit within the sheet’s margins (Margins) or the sheet’s extents (Sheet).

Margin groupbox allows you to establish where your border appears on the sheet in terms of distance from the sheet extents. You can set the border’s line font and thickness. Also, there is an option to allows you to include double-line border called Double-line border.

Independent Border groupbox is a less commonly used option that allows you to place your borders separately from margins. This is only useful if you have unusual distribution of sheet zones that do not take the border into account, with the same Right, Left, Top and Bottom settings as Margins.

Zone Formatting

Zone Formatting groupbox provides several highly specific settings to control the display of zones within the border.

You have the option to show or hide zone dividers with the Show zone dividers option. With this option off, the lines that represent the divisions between zones do not appear on the border.

Show zone dividers is checked
Show zone dividers is unchecked

In Zone Formatting groupbox when Show zone dividers is checked, you can control the line font, line thickness, length for the dividers.

There are also settings under Center zone divider that allow you to control the center zone divider’s length in both directions from the border.

Use Center zone divider settings to control the length of the center zone divider in both directions from the border.
If you do not want center zone divider to extend into the drafting area of your drawing, you can input 0 (zero) into the second field.

Under Zone labels, you will find several options and settings that allow you to control the visibility, placement and font of the letters and numbers which label your zone columns and rows.


Finally, you can even set a layer upon which your border should be placed within the Layer groupbox.


Once you have made all your choices for options and settings on this page of the PropertyManager, you can choose OK button to accept, or you can continue on to the next page for one more advanced function.

Mask Area to Remove some Zone Formatting

Page 3 of the Automatic Border PropertyManager allows you to create one or more masks for your border. A mask is an area on your border where you wish to remove zone labels and dividers. Typically, you will use masks to create space outside your margins to add a company’s legal notice or (if you are still plotting your drawings) you can add part number, sheet number or other information to quickly index through a pile of drawings.

To create a mask, click on the plus sign button.

When you click on the plus sign button, a box will appear on the Sheet Format. You can modify the size and location of this box using the grips.

For example, if you wish to add your company’s copyright notice to the upper left, move and resize the box to cover the upper left corner of your border.

You can add more than one mask. Each mask that you create will appear in the PropertyManager.

All Done!

When you select OK, you accept all the changes that you’ve made to your border, including the masked area. You will still be in the Sheet Format mode. Add any additional details you wish for your Sheet Format.

Return to your drawing’s Sheet mode by selecting Edit Sheet Format one more time.

Your changes will now be the background to your drawing.

If you wish to reuse your newly edited Sheet Format, use the Save Sheet Format command. Find this command in the File pulldown menu, shown above.

Automatic Border tool simplifies a task that can be a tedious sketching exercise. Not only does the above functionality allow you quickly create the drawing border that you want, you can easily edit your drawing border as the need arises.

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.