This is the second of my dive into DimXpert for SolidWorks. If you missed it, the first can be found here
In review… DimXpert provides an environment to add dimensions to your 3D Models, complete with tolerancing. It can check your work for “dimensional completeness“
DimXpert defaults with certain settings, which are adjustable in the Document Properties. Go into the Options, Document Properties tab and within the Drafting Standard section you’ll find the DimXpert portion. This is what sets the defaults and the appearance of your dimensions and annotations for when you use DimXpert. By picking DimXpert, you’ll reveal the general settings. In this area set the standard, the method (block tolerance or general tolerance), and default values for the method chosen.
The sub-options provide additional details for configuring DimXpert with more specifics than the general settings found on the DimXpert page.
Remember that the tab is labeled Document Properties meaning that changes only apply to the active document. You’ll want to update your template(s) with the changes you want to use all the time.
I know what you are probably thinking… anything a computer does automatically it almost always does it automatically wrong! I would normally agree with you but remember that DimXpert was purposely built for mechanical / manufacturing dimensioning and detailing. It recognizes features, not geometry, and it is standards based. So, when you want to tempt fate and let Solidworks do the heavy lifting for you, use the Auto Dimension Scheme feature. Auto Dimension Scheme does as advertised. It automatically applies dimensions and tolerances to your part based on the features it finds and how you have the settings configured in the Document Properties.
There are two steps to take before running the feature… #1 configure the settings in the Document Properties, #2 add the datums to your model (if required). Auto Dim will analysis the model’s features, any existing dimensions, and then work to fully define (constrain) the model. It may not result in a full constrained dimensioning scheme, so you may have to manually add a few dimensions.
After starting the command, adjust the settings as required. Is the part prismatic or turned? Do you want a tolerance type of Plus / Minus or Geometric? Is the default patterning type linear or polar?
Next select the Reference Features in the form of the primary and optional secondary and tertiary datums. Finally set the scope, are you dimensioning all features or just selected.
Accept it and Solidworks creates the dimensions and annotations. When complete the dimensions can be adjusted in both position and properties as if created manually.
You are now rocking at adding the dimensions and other annotations… but what’s next? How do we share this information with others? Sticking with the 3D annotation idea you can generate an eDrawing.
To create an eDrawing select Publish to eDrawing from the File menu. The screen flashes as it captures each view and then it launches the new file in the eDrawing application. The great thing about eDrawings? The viewer is free AND as you switch between views annotations are automatically turned off when they do not lie in the view plane.
I know, there will still be times when you need a good-old-2D-drawing… but don’t fear, you do not need to duplicate your efforts. When creating views of parts annotated by DimXpert the annotations transfer into the drawing. So even though you might need to move things around slightly, you’ll be guaranteed to have everything [Just make sure to enable the DimXpert option]
See it in Action
The last icon is to perform a tolerance analysis with TolAnalyst (a premium feature). With this, you’ll be able to “quickly verify dimensioning and tolerancing schemes to ensure proper fit and function“. It is intended for assemblies and I’ll cover it in a future post.
Feature Image “Man with an Abacus and a Book”