Dessins : Dimension Précision Dépannage

Article by Robert Gemmell updated July 7, 2023

Article

Drawings are crucial for communicating the precise dimensions of your part and/or assembly. Understanding and controlling precision is therefore critically important. Users can easily find it frustrating and confusing when trying to manipulate these values. In this blog, we will look at some dimension precision troubleshooting.

Let’s first take a look at four places where precision can be controlled.

  1. Templates, often your company will have these precisions preset so you don’t have to worry about them. If your company doesn’t have templates set up there is a great opportunity to learn how to make your own set of templates in the Drawings course!
  2. Document properties, this is where all the precision is set by default, and also what templates use to customize the defaults, this will affect all dimensions in the drawing.
  3. Property manager, you can select single or multiple dimensions to modify precision.
  4. Dimension Palette in-context popup.

Knowing where we can change the dimensions doesn’t always give us the results we need so I’m going to go over four common scenarios you may experience when considering dimension precision.

  1. Dimensions are using the wrong units.
    • You can quickly change the Unit System in the bottom right of the SOLIDWORKS window in the status bar.
    • You could also verify that the units are set up correctly for the template by going to Tools > Options > Document Properties > Units and selecting the correct Unit System.
  2. Dimensions aren’t following the expected standards or you want all the dimensions in the drawing modified.
    • The first thing to consider is if the dimensions are using the defaults. If the dimensions have been changed using the property manager they will not be affected by changes to the document properties. You can force these dimensions to start using the document settings by changing the precision in the property manager to “Document”.  This will link it back to the document properties and also give you a preview of what the document properties currently are right before “(Document)
      • Click on a dimension and use the Tolerance/Precision section of the Property Manager.
      • Click on the dimension and cursor over the “Dimension Palette” icon and select Precision from there.
    • Ensure the Document Properties are set up correctly.  To do this, go to Tools > Options > Document Properties > Dimensions (You may have to find your specific dimension type) >Primary Precision and verify that it’s correct.
  3. You wanted to see a “0” before the decimals when the value is less than 1.
    • These options can be controlled in Tools > Options > Document Properties > Dimensions > Fractional Display > Check the box “Include leading zero for values less than 1.
  4. You don’t want to see trailing zero’s when you have a whole number.
    • Tools > Options > Document Properties > Dimensions > Zeroes > Trailing zeroes and change the options to your preference.
    • If there are specific dimensions that should be different from the default you can change these using the precision options discussed in 2. Dimensions that aren’t following the expected standards.

In summary, troubleshooting incorrect dimension precision in a SOLIDWORKS drawing involves making sure your template/document properties are setup correctly and making sure specific dimension changes are done using the Property Manager or Dimension palette.  I encourage you to take a look at some of the other options you can control in the property manager under dimensions and note there is a drop down to specify different types of dimensions.

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Robert Gemmell

Robert est consultant en formation et en processus SOLIDWORKS.