How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part 4
In this last part of our series on SOLIDWORKS MBD (Model Based Definition), we will explore how it can intelligently show and hide 3D annotations while you are rotating the model to give you extra clarity while still respecting all the critical-to-function annotations. We will also see how to publish models as 3D PDF files or eDrawings files. These widely accepted file formats are often used in existing processes. eDrawings Viewer is a free viewer that opens eDrawings files. There are a variety of free tools including Adobe™ Reader that can be used to view 3D PDF files. In addition to providing associative information such as engineering notes, BOM, and rich Meta properties, you can also explore the model in 3D with Pan, Zoom, Rotate, Measure, Section, and other 3D tools.
SOLIDWORKS MBD Dynamic Annotation Views
All of us are used to the standard drawing views of a drawing: front, top, side, and isometric. But how does that work in SOLIDWORKS MBD (Model Based Definition) if we do not have a drawing. Don’t all of the annotations from each view get in the way of each other? Find out how Dynamic Annotation Views keeps this from happening in SOLIDWORKS MBD. Let’s take a quick look at this sample gear plate that has all of the necessary dimensions added using SOLIDWORKS MBD. As you can see, all of the dimensions are showing and are pretty much unreadable because they all overlap each other.
On the SOLIDWORKS MBD toolbar is the Dynamic Annotation Views button. Note: You can also access this tool by right-clicking Annotations in the FeatureManager design tree.
When Dynamic Annotation Views is activated, only the annotation views that are relevant to the current model orientation are visible. So, as shown below, the mess of dimensions we just saw above is now barely seen as you rotate the model.
As you rotate the model to a view that has dimensions (in this case, the front view), the faded dimensions appear normal again.
After you rotate pass that view, the dimensions fade away again. Very cool!
One additional trick to note is that the annotation types you are going to see as you rotate the model using Dynamic Annotation Views depend on the annotation types that are selected on the Annotations shortcut menu or Annotation Properties dialog box.
These options are: Show Feature Dimensions, Show Reference Dimensions, Show DimXpert Annotations, and Show Reference Annotations, which displays annotations that are not dimensions like reference dimensions, balloons, surface finish symbols, weld symbols, geometric tolerance symbols, datum feature symbols, and datum targets.
The option Show All Views in Dynamic View Mode does exactly what it sounds like. If this option is selected, all annotation views regardless of their show/hide state in the Annotations folder of the FeatureManager design tree are shown. If this option is cleared, only annotation views that are not hidden are shown.
How to Publish SOLIDWORKS MDB Models as 3D PDF Files
Does everyone on the shop floor need SOLIDWORKS if we are not going to be printing out any prints? That’s a good question. Unlike traditional 2D drawings, SOLIDWORKS MBD guides the manufacturing process directly in 3D. There are a couple options to be able to view these models outside of SOLIDWORKS. One of them is a 3D PDF file. Many companies communicate information using the PDF format. In fact, Adobe Reader is free and is already installed on 93% of internet-connected computers, according to Adobe. SOLIDWORKS MBD allows you to publish all of the rich manufacturing information to 3D PDF in a simple and repeatable manner.
3D PDF is a very convenient way to share engineering quality 3D data. But don’t we already have Save as 3D PDF in SOLIDWORKS? Yep. But the SOLIDWORKS MBD Publish to 3D PDF allows you to do more. Both support PRC Data Format (ISO certification pending) and B-Rep Data (accurate for measuring and machining). But only SOLIDWORKS MBD supports 3D Product and Manufacturing Information (PMI), Bill Of Materials (BOM), Customizable Templates, Multiple-Configuration Support, Display States, and Product Views (3D Views, Named Views, Predefined View Orientations)
Select Publish to 3D PDF in either the SOLIDWORKS MBD toolbar or the 3D Views pane to create a sharable 3D PDF presentation. The process is pretty straight forward. You pick a template. The software comes complete with a library of PDF templates that you can easily customize or you can you can create your own for assemblies as well as parts. For more information on templates, see How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part2.
Then, you pick what Views to Include, which includes the standard views and any additional defined SOLIDWORKS MBD views that you may have created. You can also view the custom properties which will be passed directly into the PDF file.
Choose a file name and path where you want the file saved. There is an option that lets you include custom text fields. Lastly, a check box allows you to view the PDF after saving. When you view the 3D PDF you can see the values for the custom properties are automatically populated. All of the 3D Views previously created in SOLIDWORKS are available as well.
It is very easy to navigate through the design. When you select dimensions, the reference geometry is highlighted, making it easy to see which dimensions belong to which faces. Comments can be added to the text field of the PDF file and then sent back to engineering. This simple capability can really help collaboration with the supply chain. So, creating 3D PDFs is very fast and flexible with the purpose of reducing the common errors associated with interpreting 2D drawings. If any changes are needed, you can update your model and pass on critical information quickly and easily without creating a new 2D drawing. With an assembly PDF, you will see an accurate Bill of Material. The PDF is very interactive. Select an item in the BOM and it highlights in the 3D graphics area and vice versa.
How to Publish SOLIDWORKS MDB Models in eDrawings
How can my supply chain work with my models if they don’t have SOLIDWORKS? Many companies rely on eDrawings to convey product information and you can easily publish SOLIDWORKS MBD into this format. You can choose whether to include some or all of the configurations and SOLIDWORKS takes care of the rest. Suppliers can easily review your rich MBD data in eDrawings format using a free eDrawings viewer. To publish a model to eDrawings, simply click Publish eDrawings File in either the SOLIDWORKS MBD toolbar or the 3D Views pane. Note: If there are multiple configurations of the model, you can select which configurations you want to publish.
The document opens in eDrawings. After you set your options, click File > Save to save the document in eDrawings. eDrawings also allows you to view and manipulate all of the 3D views created earlier. Selecting a dimension highlights the geometry references, making it very easy to understand the model without the need for a 2D drawing.
SOLIDWORKS MBD provides some great new tools for the creation, organization and output of Product Manufacturing Information and really helps streamline Production, cut cycle times and improve product quality.
We hope this series gives you some good insight to the new SOLIDWORKS MBD product. Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SOLIDWORKS tools. All of these articles will be stored in the category of Daily Dose…..of SOLIDWORKS Support and links to each article with their release date are listed below:
- How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part 1 (Bryan Pawlak 3/2/15)
- How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part 2 (John Van Engen 3/3/15)
- How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part 3 (Blake Cokinis 3/4/15)
- How to Eliminate 2D Drawings with SOLIDWORKS MBD – Part 4 (Neil Bucalo 3/5/15)
Neil Bucalo, CSWP, CSWS-MD
Computer Aided Technology, Inc.