What’s New with Drawings in SOLIDWORKS 2018

While many SOLIDWORKS users are focusing on some of the more whiz-bang features in the SOLIDWORKS 2018 release, they might be missing some of the cooler upgrades in the drawing module. Like it or not, most industry still relies on 2D drawings for quotes, fabrication and inspection.

The 2017 SOLIDWORKS release introduced Advanced Holes. Advanced holes are multi-step holes. Prior to the 2017 release, if you wanted to place a counterbore hole on both near and far sides of a machined part, you would have to place the hole on each side and then modify the hole callout to indicate each hole. In 2017, you could place the multi-step hole using the advanced hole feature (located under the Hole Wizard), but you still needed to modify the hole callout.

The 2018 release has now caught up, and when you have placed a multi-step hole with the Advanced Hole tool, the hole callout tool will show both near- and far-side holes without you having to make any edits.

The hole callout now properly calls out advanced holes in the 2018 release.

You also have considerable control over how the hole callout is displayed by reversing the callout order or switching the near- and far-side callouts. To modify the order used in the hole callout, simply select and enable/disable the options in the Properties panel.

Hole callout options for advanced holes.

2018 provides more flexibility in controlling how hatching is displayed in section views.

You can use layers to designate the color of the hatch as well as define the hatch pattern, color and scale. You also have the ability to create a partial section or emphasize the outline in a section.

Section view.


Section View new options in 2018.

One of my pet peeves for a lot of CAD software is their failure to comply with ANSI dimensioning standards, particularly leading and trailing zeros. The 2018 release of SOLIDWORKS finally has given the users the ability to fully control how trailing zeros are managed by allowing users to set their preferences in the Document Properties. Simply go to Options, Document Properties, Dimensions and make your selections.

Controlling leading and trailing zeros.

Users should be aware that “Smart” or “Standard” are no longer valid selections in 2018, and you will get an error message if you pick those options. Instead, you are required to select whether you want the zero to show or remove. The ANSI standard is to remove leading zeros on imperial dimensions and show them on metric dimensions. Whether or not you display trailing dimensions in either unit is based on your tolerance requirements.

Once you have figured out what units you are working in and your tolerance design requirements, I recommend you save your preferences to a template, so you don’t have to worry about having to make this setting for every drawing.

2018 adds the ability to create a broken-out section view of an existing section view. The tool is available on the View Layout ribbon or on the right-click shortcut menu when selecting a section view.

The new Broken-out Section tool.

This tool is useful when you have a machined part, casting or injected molded part that has interior features that are not easily dimensioned or visible in standard views. The method of creating a broken-out section view is similar to creating a cropped view or broken-out view. You select the view and create a closed polyline sketch, using the sketch tools, then select the tool either from the ribbon or the right-click menu. I recommend you enable the Preview option so you can determine whether you have specified the correct depth for the section view.

Broken-out Section view options.

2018 introduces the ability to create a drawing view that displays alternate positions of an assembly that has moving parts. This is a nice way to show the range of motion or to display a motion study of an assembly. In order to create the view, you first need to create a configuration inside the assembly file of each position in the assembly you want to display. For each configuration, you will want to configure the controlling mate to define the desired position in the assembly. This can be challenging for novice users who are just learning how to use configurations and assign mates correctly.

For example, I have this assembly of a set of pliers. I want to show how far they open and close.

Pliers assembly.

I am controlling the position of the plier jaws using an angle mate.

Plier mates.

The Angle1 mate is the total angle between the two grips. The Angle2 mate is between the top grip and the top plane. The value of the Angle2 mate is half the value of the Angle1 mate.

The angle mate definitions.

Next, you need to go to the Configuration Manager to create a configuration for each position you want displayed in the view. Highlight the top level of the assembly, right-click and select Add Configuration. Name the configuration something meaningful to make it easy for you to identify if you need to make any changes.

Adding a configuration in the Configuration Manager.

Suppress the angle mates for the original configuration and create a set of mates for each position configuration. Select the mate, right-click and select Configure Feature.

Suppress the mates for their corresponding configuration.

Once you have set up the different configurations and what position you want the assembly to be in for each configuration, you can create the alternate position view in a drawing.

Place the initial view or base view for the alternate position in the drawing.

Place the initial position view.

Select the Alternate Position view tool from the View Layout ribbon or by selecting the view and right-clicking to access the Drawing View shortcut menu.

The Alternate Position View tool.

Then select the desired configuration to use for the next alternate position from the Properties panel. You can create a new configuration on the fly using the Properties panel, but that only works if your model is underconstrained. If you use the New Configuration option, do not apply any mates controlling movement to your assembly. Instead, you will drag the components to the desired position for each configuration. I don’t really recommend this method because it may or may not reflect how the assembly will actually work.

The Alternate Position view properties dialog.

The alternative view position is then overlaid on top of the original view.

 Alternative view position.

 I have left the most popular new drawing feature for last. I recently attended a SOLIDWORKS 2018 launch event hosted by SOLIDWORKS reseller GoEngineer. This feature garnered the most applause of all the new features in the 2018 release.

The Parts List formatting tool bar now includes a tool that will automatically convert all text in the parts list to uppercase, so your bill of materials (BOM) will now comply with ANSI standards, without you having to go through all the part properties used in the BOM and re-editing the text. To access this tool, simply left click on the upper-left Move icon after selecting the parts list.

This is probably one of the more time-consuming tasks that has been inflicted on users when creating assembly drawings.The 2018 release now liberates users to focus on more important tasks.

Convert all text to uppercase.

So, there you have it. The six new drawing improvements in SOLIDWORKS 2018 are:

  • Hole callout for advanced holes,
  • Control of hatch properties in section views,
  • Control of leading and trailing zeros in dimensions,
  • Creating of broken-out sections,
  • Alternate position views and
  • Automatic uppercase text in parts lists.

These improvements combined with the other new features introduced in SOLIDWORKS 2018 should make users consider an upgrade to this release sooner rather than later.

About the Author

Elise Moss has been using SOLIDWORKS since 1996. She is a Certified Solidworks Professional and a Certified Solidworks Educator. She teaches SOLIDWORKS at Laney College in Oakland, Calif. She has a BSME from SJSU and owns her own consulting firm, Moss Designs, in San Jose, Calif.

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