Manufacturing

Extending Product Manufacturing Information to 2D Drawings (On the Edge Solid Edge Tutorial)

1 Mar, 2008 By: Russell Brook

Solid Edge is able to include PMI dimensions already defined in 3D models on your 2D drawings.


Previously in this column, I wrote about adding product manufacturing information (PMI) to models in Solid Edge. To recap, PMI is a way to add geometric dimensioning and tolerancing (GD&T) symbols to 3D models. By annotating models in this way, you im-prove productivity, ensure the 3D information is accurate, and reduce reliance on 2D drawings during design reviews.

 

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PMI from 3D models can be included on 2D drawings.

So does PMI spell an end to 2D drawings? No, but it does remove the need to update multiple documents while a design is still evolving, and many companies still rely on 2D drawings for documentation, inspection, quality control, and more. So whether you use hard copy or electronic drawings, they will be around for some time yet because draw-ings are easy to file, different departments have easy access to them, and they are traceable. Models with 3D PMI annotations are designed for streamlining the manufac-turing process, but drawings often are needed to inspect finished components.

Adding PMI to a 3D model also makes sense from a design perspective because critical dimensions and manufacturing information is captured as you design. Also you are add-ing this information to a single model, unlike orthographic drawings where dimensions need to be spread across several views to relay your design intent.

To speed up drawing production, Solid Edge now allows you to include PMI dimensions already defined on 3D models in 2D draft mode. Just save relevant model views with your 3D model that you want to represent on your drawing.

 

Using PMI in 2D
Before I discuss how to create drawings that include PMI, here are some more capabili-ties regarding PMI in 2D:

  • Drawings that include PMI can be created in both draft-quality and high-quality draw-ing views.

     

  • View orientation is defined by your saved model view (it's good practice to use mea-ningful names as you create them) along with visible components if you are working on an assembly file.

     

  • You can add more model views to your model if later you find another view, angle, or perspective is required.

     

  • You are able to continue annotating a drawing view as you would if you had not cho-sen to include PMI.

     

  • You can set Quick Sheet templates to further speed up drawing production.

     

  • If you add a prefix or tolerance to a PMI dimension in 3D, you will be notified on the drawing.

     

  • Dimensions are associative, so changing your model updates the 3D PMI dimension, which in return updates the drawing.

     

  • At the time of writing, PMI annotations such as callout labels and balloons are not displayed on the drawing; this is planned in a future release of Solid Edge.

How to Create a Drawing View, Including PMI Dimensions
To continue with this quick tutorial, you need to have a model that includes PMI and to save some model views within that file. If you are unsure how to create PMI annotations in 3D please refer to my previous article on PMI.

While in the 3D model, choose Model View from the PMI toolbar.

 

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Click on the Model View icon to save a view using current display.

Fill in the Model View dialog box and repeat for any subsequent views you want to rep-resent.

 

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Model View Options dialog box.

Tip: Save orthographic views (top, side, end) and an isometric view. You can also in-clude cutaway views.

Start a new drawing using the Drawing View Creation wizard. Solid Edge will recognize if there are any PMI dimensions to include.

Select the check box Include PMI Dimensions from Model Views to include dimensions. Dimensions will be ignored if you do not select this option. In some circumstances this might be desirable.

 

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The Drawing View Creation wizard.

Simply place your drawing views. Notice PMI dimensions are included.

 

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A Solid Edge drawing that includes PMI dimensions.

After a model view with PMI has been placed, the PMI can be turned off through the View Properties dialog box.

 

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The General tab in the View Properties dialog box allows you to turn on or off PMI dimensions.

The Configuration box has been enhanced to include model views, allowing you to choose other views after placement.

 

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In View Properties dialog box, the Display tab allows you to choose a different view.

Conclusion
That's all there is to it. As you can see from my example, you can show assemblies (as well as single parts), individual part colors, and section views and more.

See you On the Edge next time.


About the Author: Russell Brook

Russell Brook

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