Because I spent over a decade of my life as a drafter, dimensioning schemes are one of my favorite topics. When I am discussing how to create drawing, it’s always a little surprising to me how many people don’t know the difference between model items and smart dimensions. So, let’s take a look at SOLIDWORKS Model Items and get down to what they are and when we can use them.
What are SOLIDWORKS Model Items?
Model Items are dimensions, annotations, or reference geometry items located inside of our part and assembly files that we can reuse on drawings. For example, we start a part file and create a 2D sketch of a rectangle. We then fully define that sketch with two dimensions and use extrude to create a box. The dimensions we used to define and create the feature are model items we can show on a view inside of a 2D drawing.
Who can benefit from using Model Items?
Designers who want to save time creating their 2D drawings can really benefit from using model items. If the person who makes the 3D model keeps the design intent of reusing dimensions in the 2D drawing in mind while modeling, they won’t have to redefine any features when creating the drawing. It is a much faster way to define 2D views on drawings.
How do we use Model Items?
In a 2D drawing in SOLIDWORKS, under the annotation tab, the second icon you will see is Model Items. When you have activated this icon, our Model Items menu is going to ask a few things. First is going to be the Source and location. The Source option allows you to select specific features to import their items or import everything from the entire file. The Location option is going to let you choose what views to import the model items in from.
The next options we are asked about is what type of items do we want to import into the drawing. Dimensions you add in part files are automatically “Marked for Drawing”. You can turn this off by right clicking on your dimension in the part file, and the color of the dim will change to purple. This option allows us when 3D modeling to make sure certain dimensions that are for reference won’t get pulled into the drawing with everything else. Going back to our drawing, looking back at Model Item Properties, the first options under dimensions are to import dimensions that are marked for drawings. The second option is to import dimensions that are not marked for drawings, so if you end up needing that purple dimension, you can still import it.
The second line of options for dimensions are for hole wizard. When creating a hole wizard feature, two sketches are made: the hole shape and the location. Model Items gives us the option to import dimensions from these two sketches. Something cool it can do is make a hole callout instead of just importing linear dimensions as well with the file icon.
The other sets of items are Annotations (For example: notes, Geometric Tolerance Blocks, and weldment callouts) or reference geometry (reference planes, curves, or routing points) that we can pull from the model into our drawings just like the dimensions. These items are useful to have, and again if we are already using them in our part, why not reuse them for our drawings.
Tips for using Model Items
When importing dimensions, sometimes we import way more then we mean to. When you select your features and bring in your items, you have the ability to right click on the preview of them and shut certain items off manually. They will be light grey until you click the green check, and then it will disappear.
Another thing to note is that sometimes SOLIDWORKS will guess the wrong view to put your dimension on. Your overall may be on the TOP view when you rather it on the FRONT. You can easily move dimensions around by holding the shift key and dragging your dimensions to a different view.
Model items are pulling the same dimension from your part file into your drawing file. Because we have this connectivity between the two files, we can actually change that dimension by double clicking on it in the drawing. When I change it in the drawing, I am also changing it in the model. This is useful for making revisions and not something you can do with Smart Dimensions.
When not to use Model Items
You cannot add Model Items in Detailing Mode. Detailing Mode allows us to open very complex and large drawings very quickly by not fully loading the model’s file. Because Model Items are directly pulled from the file, the option is greyed out.
There’s more to dimensioning then just measuring lines. SOLIDWORKS Model Items is a powerful tool that can drastically speed up your drawing time and take out repeating steps you don’t need to do.
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