Sketch text can be used to speed up your design, learn how to use it in this quick article!
Cupid has struck me and in honor of Valentine’s Day, I am going to design the iconic candy conversation hearts!
I already built the candy heart solid body and now I’m ready to add the conversation portion of the design. The lettering on our candy hearts will allow us to discuss Sketch Text and the useful, or in this case romantic, ways it can be used in SOLIDWORKS.
SOLIDWORKS makes it easy to add text to your parts through Sketch Text. Start by creating a sketch on the surface you wish to add text to.
For my candy heart, I will choose the top surface of the body. Once you are in a sketch you can select the Text shortcut on the CommandManager sketch tab or go to Tools > Sketch Tools > Sketch Entities > Text. The Sketch Text property manager will open.
The first group box in the property manager is labeled Curves and is used for positioning the text. An edge, curve, sketch, or sketch entities can be selected here to help position the text. If you are using a sketch entity in your current sketch, be sure it is construction geometry so it is not included when the text is referenced later.
The Curves group box can also be left blank, which will cause SOLIDWORKS to create a construction point next to the text for positioning after the text is created. The construction point can be positioned using dimensions or relationships and will not appear when the sketch is referenced later. We will add construction geometry to the sketch to center our text on the heart, however, sketch entities cannot be created while in the Sketch Text property manager. We will need to exit out, create our reference geometry, and then start the Sketch Text feature again in order to do this.
The second group box in the property manager is labeled Text and is for the text itself. There are two main things being controlling from here: the text body and how it should be displayed.
The text body can be typed into the text box, and will appear in the graphics area as it is entered. File properties can also be linked into the text body using the Link to Property icon. There are options for rotating, aligning, mirroring, scaling, and spacing the text. The default font can be applied, by checking the box, or customized, by unchecking the box and selecting the Font button, which will become active. Here you can choose from all the true type fonts, font styles, and sizes available on system.
My default template font is not right for our candy heart so I am going to uncheck this box and customize my text. A common font used with Sketch Text is OLFSimpleSansOC Regular, which is the stick or single line format font for SOLIDWORKS. In many applications where text is laser engraved, water jetted, or CNC machined this font will be required. I will not require the stick font for manufacturing my candy hearts and will use a smaller font with round bold lettering.
Once the Sketch Text is created, it acts similar to a block. Selecting or hovering over any entity of the text will show the text icon next to the cursor and highlight the entire text body created from the same command. The text can be edited with a double click or right clicking and selecting Properties. If you would prefer the Sketch text to not behave like a block, it can be broken down into its separate sketch entities by right clicking and choosing to “dissolve sketch text.” Dissolving the sketch text will no longer allow you to make changes to the text.
When selected for a feature, the sketch text will act as an entire entity and contours do not need to be applied. The most common features used with Sketch Text would be an Extrude Boss/Base, Extrude Cut, or Wrap. The messages on my candy hearts will be manufactured by a stamp; therefore, I will use an Extruded Cut to press the letters into my heart.
Features can be given their own display settings. This can be helpful when Sketch Text has been applied to make the lettering standout. There are several ways to apply unique display settings to a feature. One method is to expand the display pane of the FeatureManager and select the display icon in line with the component you wish to alter. I am going to make the messages on my candy hearts red so I will choose the appearances icon and the desired color.
I have now finished my first candy heart; however, there cannot be just one candy heart! That is the fun of the whole thing. There needs to be a whole variety of colors and messages. Configurations and display states are the perfect applications to create this family of candy hearts composed of text and color combinations.
Configurations allow multiple variations of a part or assembly model in a single document. There are several ways to control configurations, one of which is the Modify Configurations dialog box. This method uses a table format to create and modify all the configurations from one easy location. To create the Modify Configurations dialogue box in a part file, right click on a dimension, feature, or material. The Modify Configurations dialogue box will open with a column for the parameter it was created from.
Configurations can be added, removed, and modified from the Modification Configuration dialogue box. I created five other configurations of the candy heart by typing in the desired names into the “creates a new configuration” row of the table.
Parameters can also be added, removed, and modified from the Modification Configuration dialogue box. The only parameter I want to configure is the text. Text cannot be directly configured; however, it can configured indirectly through file properties, which we already know can link to sketch text. In the Modify Configurations dialogue box there is a button to add a file property. Clicking this creates a new column in the table for file properties. An existing property can be referenced using the drop down next to the header, Custom Properties, but a new property can be created by double clicking the sub header, New Property.
I created a new property called Heart Text and filled in the desired phrases I wanted to appear on the candy hearts. Now that I have more than one column I can delete the original column used to create the table. One column is the minimum number that can exist in the design table. I will now want to give my configuration table a name and save it. Saving the table adds a folder to the top of my ConfigurationManager tree, which holds the table and allows me to access it again later.
The custom property, Heart Text, needs to be linked to the Sketch Text. We will need to edit sketch, and double click the Sketch Text to make a modification. We will clear out the original text, select the file property icon, and choose our newly created custom property Heart Text. A piece of syntax is added to the text group box to represent this custom property. Choosing OK applies the change to all the configurations.
Rebuilding and reviewing the configurations for accuracy shows some of the configured text body is too long for the size of the heart. Instead of making the font smaller, the text will be broken into two lines. This cannot be done inside the sketch text feature or text of the file property. The text will have to be broken into two custom properties, Heart Text and Heart Text 2.
More than one custom property can be referenced in a single Sketch Text; however, in some cases a second line of text is not needed. When this happens Heart Text 2 will be empty which will cause Sketch Text to show a syntax error. To avoid seeing this we will make the second line its own feature and suppress it in the configurations when not needed.
Display states control appearances. They have the option of being linked to a configuration. Leaving a display state unlinked allows it to be shared by multiple configurations. In this way we are able to change the color of the candy heart body in any message configuration.
That gives us a total of thirty six possible different conversation hearts. We now have a part file capable of filling an entire box of candy message hearts!
And voila! Happy Valentine’s Day!