My Top 9 Favorite SOLIDWORKS Drawing Tips
Having taught SOLIDWORKS for over 16 years, I have accumulated many best practices and drawing tips that I regularly share with my students. In this article, I will share these with you in the hope that they will help you produce better drawings more quickly.
A SOLIDWORKS drawing can be broken into two major components. There is the drawing, which is often the final product of your design, and there is the drawing template, which is the base of all your drawings.
Because it is the base of your drawings, the importance of the drawing template cannot be overstated. Having a well-laid-out drawing template can ensure that drawing standards are being adhered to and that there is a clear flow of information from document to document.
The drawing template is composed of four major components:
- The template itself, which is the container for all the other components
- The document properties, which are used to define the drawing standards
- The sheet format, which is the area where we define our title block, sheet borders as well drawing zones
- The sheet properties, where we define the sheet scale, type of projection, as well as the sheet format
Document Properties and Drawing Standards
Let’s first look at the document properties. My first tip here is to make use of the Document Properties dialog. It surprises me how many times I see people use the default SOLIDWORKS Drawing Template and modify the document properties on the fly. Not only does this create additional work, but this practice inevitably leads to inconsistency between drawings.
The software ships with several drafting standards.
You can tweak or completely modify these standards to meet your company’s own standards. Once you have developed your standard, you can save it.
Saving the drawing standards you created allows you to reuse them and can safeguard against the loss of your work.
As mentioned earlier, the sheet format is where you define your title block. A well-defined title block will be aesthetically pleasing and pull existing information directly from the drawing, or from the referenced model or assembly. The sheet format can be accessed by right-clicking on a blank area of your drawing and selecting Edit Sheet Format.
One way to approve the appearance of your title block is to have the annotations centered in a region of the title block. This is accomplished by right-clicking on an annotation, selecting Snap to Rectangle Center and then selecting the lines that define the borders of the rectangle.
To ensure that your title block displays the correct information, it is best to have a central repository for this information and then link annotations in the title block to this repository. This information is typically stored in the document properties of a drawing, or in the referenced part or assembly. To link an annotation to a property, start creating a note. Do not enter any text; instead, select Link to Property from the SOLIDWORKS Property Manager.
In the Link to Property dialog box, select which document and document properties you want to attach your note to.
Linking annotations to properties can be applied to all annotations in your drawing, not just those in the title block.
Drawings border sizes and drawings zones can be created using automatic borders. Automatic borders can be accessed from the Sheet Format tab of the Command Manager.
The Automatic Border tool is a multipage wizard that allows you to define your drawing borders and establish drawings zones. Once you have established these zones, the zone information can then be added to a note from the Add Zone option of the Property Manager.
You can display the zone or just the zone column or zone row values.
Once you have finished modifying the sheet format, you can save it to the drawing template after the template has been saved. You can also save the sheet format as a separate file for later use.
When it comes to sheet properties, there are two tips I will offer. The first is to ensure that the right sheet format is being used. If you spent all that time creating your sheet format, ensure that it is the one listed in the sheet properties. The second tip is to keep in mind that you can switch the sheet size if you run out of room in your drawing. Sheet properties can be accessed by right-clicking on a blank area of your drawing and selecting Properties.
Saving the Template
Once you have modified all the areas of the drawing template, you will need to save all your work. To do this, select Save As from the File pull-down menu in SOLIDWORKS. In the Save As dialog box, select Drawing Templates from the Save as type pull-down menu.
To ensure that all SOLIDWORKS users in a company are accessing the same document templates and sheet formats, these should be stored on a common network drive. Next, the file locations for each user’s computer should be modified so that they look to this common location. File locations are set from Tools>Options>System Options>File Locations. File locations, as well as other user settings, can be copied using the Copy Settings Wizard. The saved settings from the Copy Settings Wizard can then be included in a SOLIDWORKS installation Admin Image so that these file locations are set when the software is installed.
One Component, One Drawing
Whether it is a part or an assembly, the process of tracking which drawing is associated with which model or assembly is greatly simplified by having one component as the focus of that drawing. Often I see drawings that contain the main-level assembly, all the subassemblies and all the parts in one drawing, with each component being represented in its own sheet.
This may initially seem to be a smart way of enveloping an entire project in one file, but what if some of these components are used elsewhere? Do we then create a new drawing with its own hierarchy of sheets? Obviously, this would result in multiple drawings of the same components. How do we then identify which drawing needs to be sent downstream of the design process? Which is correctly annotated? In fact, how do we find this one sheet that is buried in a drawing somewhere?
By having a simple relationship of one component and one drawing, it is easy to track the drawing and its referenced components. This can be especially useful when working in a multiuser environment, or one where data management software is used. If the drawing needs to be accessed, you can do this directly from the open, referenced part or assembly. This is done by right-clicking on the file name inside the Feature Manager and selecting Open Drawing.
Performance can always be a challenge with drawings. Not only can large assembly drawings tax your CPU and consume RAM, but all the line work in a drawing can also overload your video card. While you can go out and purchase a more capable system, there are things you can do to address this without having to spend your money on a new computer.
The first thing you can do is to work from your local drive. While network drives can be fast, they do not approach the performance of most computers. If you need to have these files accessible to multiple people, look for a data management solution. With these solutions, you work from your hard drive, but you can check your work into a centralized location, so that others can access it.
When opening a multi-sheet drawing, you can choose which sheets to load. This will reduce open, rebuild and save times. This option is available from Open dialog box.
Large Assembly Mode can increase performance by reducing the amount of information that is being loaded when you open a drawing. This can also reduce open, rebuild and save times. Large Assembly Mode can be enabled from Tools>Options>System Options>Assemblies.
Detached drawings can increase performance by disassociating the drawing from its referenced component. With a detached drawing, you can still create derived drawing view and add dimensions and notes. A detached drawing can be created from the Save As dialog box.
In some cases, it can be easier to create a drawing view in the model or assembly. This view can be saved and later inserted into a drawing. Drawing views are created in the View Orientation dialog box. One way to access this tool is by pressing the space bar on your computer keyboard.
The newly created views will appear in the View Pallet of the software’s Task pane.
Another way of achieving the orientation you want is to use the Relative View tool. This is available from the drawing and allows you to orient your view by selecting model geometry. This tool will also allow you to isolate a body in a multiple-body part, such as a weldment.
If you create an auxiliary view that is tilted, you can fix the alignment by right-clicking on the view and selecting Align Drawing View.
Checking Your Drawing
The Design Checker might be one of the most underused tools in the SOLIDWORKS suite, but it can be invaluable in catching variances from your drawing standards. The Design Checker is available from the Evaluate tab of the Command Manager. There are tools to build your checks, which can be run on drawings as well as other document types. Design Checker is only available with SOLIDWORKS Professional and Premium.
In this article, I have covered some of my favorite tips and best practices. I encourage you try these. I am confident that they will help you to create more robust and efficient drawings.
For more tips on drawings, visit the SOLIDWORKS website.
About the Author
Joe Medeiros is a Senior Applications Engineer at Javelin Technologies, a SOLIDWORKS reseller servicing customers throughout Canada. Joe has been involved with SOLIDWORKS since 1996. An award-winning blogger, he regularly writes about SOLIDWORKS products.