With every release, SOLIDWORKS introduces a number of enhancements to help you become more productive.
In this article, we will review a selection of drawing enhancements that were released in SOLIDWORKS 2014 through 2016. Most of what is in this article is available from the Help drop-down menu under What’s New.
SOLIDWORKS 2014
Reattach Balloons: Balloons, including dangling balloons, can be reattached to another component within the same drawing view. To reattach a balloon, right-click on the balloon, select Reattach and then select what you want to attach the balloon to.
Reattaching a dangling dimension.
Saving BOM Sort Settings: If you regularly sort your bill of materials (BOM) by the same criteria, you can now save for reuse by selecting “Save current sort settings.”
Saving BOM sort settings.
Angular Running Dimension: This is a group of dimensions that are measured from a selected zero position. This tool is similar to ordinate dimensions, which are used for linear dimensions.
On the left is the Angular Running Dimension, accessed from the “S” shortcut key. On the right is the result from this command.
Like the Ordinate Dimension tool, there are a number of options for displaying angular running dimensions.
Finding Virtual Sharps while Dimensioning: While dimensioning, right-click on the model geometry for which you want to find the intersection and select Find Intersection. Next, select the model geometry that would form the intersection.
The Find Intersection tool: The virtual sharp can be seen to the left of the dialogue box.
Virtual sharps can also be found in a sketch by using the same procedure used in a drawing.
Attaching Annotations to a Drawing View or a Drawing Sheet: By right-clicking on an annotation and selecting Attach, you can choose to attach an annotation to a view or the drawing sheet. If you are attaching a note to the drawing view, select the view after selecting Attach.
The Attach to View option.
Out-of-Date Drawing Views: Dimensions and annotations can be added to drawing views that are out of date. This allows you to add dimensions and annotations to drawing views without having to rebuild the drawing, which can be a timesaver for complex or large drawing views. The display of out-of-date drawing views has been changed to make it easy to add dimensions and annotations to drawing views.
Replace Model for Drawing Views: Similar to the Replace Model tool found in assemblies, drawing references can be changed for individual drawing views while the drawing is open. This option is available from the Tools drop-down menu and the Drawing toolbar or by right-clicking on the drawing view.
Replace Model dialogue box.
Setting Annotations to Display in Upper Case: Annotations can be set to display in upper case. This option can be found in the Property Manager window, which is located in the Text Format section.
Text Format is set to use All uppercase.
The Shift + F3 keyboard combination can also be used to set annotations to “All uppercase.” Select the annotation you want to change and then press Shift + F3.
“All uppercase” can also be set as a document setting from Tools > Options > Document Properties > Drafting Standard. Here there is an Exclusion list that allows you define what text will not be automatically set to uppercase.
All uppercase is set and the Exclusion list is defined.
SOLIDWORKS 2015
Drawing Zones: In the sheet format of a drawing, you can define zones in order to identify where drawing views and annotations reside in a drawing. An example would be to identify the zone where a parent view is located. To define drawing zones, edit the sheet format, right-click on the blank section of the sheet and choose Properties. Next, click on the Zone Parameters tab and define the zone size and margins.
Defining zone parameters.
Additional zone parameters can be defined from Tools > Options > Document Properties > Drawing Sheets or by clicking on Go to Drawing Sheet Properties.
Zone parameters in the Document Properties tab.
Zone lines can be shown from the View drop-down menu to make it easier to identify the zone boundaries.
Showing zone lines.
Adding zone information to a note is done from the Property Manager by clicking on the Add Zone icon and choosing the required zone information. Zone information that can be added to a note includes column, row and drawing view information.
Adding zone information.
Zone location labels can be added to detail, section and auxiliary drawing views in order to provide the sheet and zone location of the parent.
Location label.
To add a location label to a child view, select Insert > Annotations > Location Label, define the location label settings and then select the child view.
Defining location label parameters.
To add a location label to a parent view, select Insert > Annotations > Location Label, define the location label settings and then select the section line, detail circle or view arrow.
Although location label options can be set for each label individually, general document settings can be set from Tools > Options > Document Properties > Annotations.
The Location Label menu in the Document Properties tab.
Center Marks: Additional center marks can be added to existing linear and circular center mark sets by right-clicking on the center mark set and selecting Add to Center Mark Set.
Dangling center marks can now be reattached. To reattach a dangling center mark, right-click on the center mark, select Reattach and on the same drawing view, select the replacement geometry.
Decimal Rounding: There are many more options when rounding dimensions, including Round half away from zero, Round half towards zero, Round half to even and Truncate without rounding. Decimal rounding behavior is set from Tools > Options > Document Properties > Units.
Decimal rounding.
Angle Dimension Capabilities: There are a number of enhancement to angular dimensions:
- Imaginary Lines, which allow you to add an angular dimension between a line and an imaginary horizontal or vertical line.
- Remove units with 0 value for deg/min and deg/min/sec, which is used with angular dimensions set to deg/min or deg/min/sec to hide or show zero value dimensions. This behavior is controlled from Tools > Options > Document Properties > Dimensions > Angle by selecting/deselecting.
- Symmetrical Angular Dimensions, which can be added without having to select a center line each time. This behavior is triggered by pressing and holding the Shift key while dimensioning.
Layers: You can choose which layers will be omitted during printed. This is done by clicking on the print icon for the layer in Layers Properties.
Setting print option in Layers Properties.
Balloon Asterisk: Now when you mouse over a balloon containing an asterisk, a caption will explain the reason for the asterisk—for example, the item has been excluded from the BOM.
Spline Leader: Spline leaders can also be added to a note. This is done from the Property Manager after creating or selecting the note.
Setting the spline leader.
New Sheet Formats: F Size (ANSI), A0 (BSI) and A0 (GB) have been added.
SOLIDWORKS 2016
Foreshortening of Linear Dimensions: Foreshortening of linear dimensions is now possible on any drawing view. To foreshorten a dimension, right-click on the dimension and select Foreshorten from the display options. The default behavior for foreshortened dimensions can be set in Tools > Options > Document Properties > Dimensions > Linear.
Foreshorten options.
Smart Dimensioning for Simple Thread Callouts: Now when the Smart Dimension tool is active, if you select the cosmetic thread of a tapped hole, a simple thread callout is created.
Hatch Patterns: New DIN ISO 128-50 crosshatch patterns have been added to the hatch tool.
Model Break View: The 3D Model Break View option can be created in assemblies or parts from Insert > Model Break View or by right-clicking on a part or assembly’s configuration and choosing New Model Break View. Once the model break view has been created, the 3D broken view can be shown in a drawing by selecting “Show in exploded or model break state” under Reference Configuration.
Model Break View in Reference Configuration.
The 3D model break view can also be shown by right-clicking on the view and selecting Properties.
Displaying model break view.
Flag Notes: Flag notes can be created to parametrically cross-reference an area or feature in a drawing to a list of annotations, such as general notes.
To create a flag note, add a note and then in the Formatting toolbar, click Number and apply as many numbers as required.
Applying number format.
Select the item number to be flagged and select Add to Flag Note Bank.
Adding note to flag note bank.
Once flag notes have been added to the flag note bank, you can now create flag note balloons. Start the Balloon command. Check Flag Note Bank in the Property Manager, select the flag note to add and then click to place the flag note.
Adding a flag note balloon.
Flag note balloons can be added to existing notes by editing the note, positioning the cursor where you want to place the flag note balloon and then selecting Flag Note Bank in the Property Manager.
Custom Property Values: Custom property values can be shared across multiple sheets. This is enabled in Tools > Options > Document Properties > Drawing Sheets. Select “Use custom property values from this sheet on all sheets” under “Multi-sheet custom properties source.”
Applying multi-sheet custom properties.
The Sheet number option identifies the parent sheet from which all custom properties are derived.
Automatic Border: This tool allows you to control all aspects of the sheet format. It’s available while editing the sheet format. Right-click on an empty section of the sheet and select Automatic Border.
Automatic Border option from the right-click menu.
On the first page, select any items you want deleted from your sheet format.
Deleting items from the Automatic Border option.
On the second page, define the sheet formats, zone size, zone formatting, borders and margins.
Defining the Automatic Border parameters.
On the third page of the Automatic Border option, you can define margin masks, which allow you to hide zone dividers and labels in the margins.
Adding margin masks.
In this article, I covered many of the drawing enhancements that have been in added in SOLIDWORKS releases 2014 to 2016. There are many more enhancements and tweaks from 2014 to 2016 as well as from earlier releases that are not covered in this article.
To fully take advantage of new functionality and tweaks to existing functionality, I recommend reviewing the What’s New documents that ship with every release of SOLIDWORKS. These can be accessed from the Help drop-down menu and is available in PDF and HTML formats. Often there are sample SOLIDWORKS files that you can use to learn the new functionality. Your efficiency in using SOLIDWORKS can be greatly enhanced by learning how to use these tools.
About the Author
Joe Medeiros is a senior applications engineer at Javelin Technologies, a SOLIDWORKS reseller servicing customers throughout Canada. Medeiros has been involved with SOLIDWORKS since 1996. He regularly blogs about the product and has won awards for his blogging.