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Can you imagine that just about everything in front of you right now has had a dimension on it at some point. Everything except that apple over there to the left. the Big Guy upstairs has an automated routing programs for that kinda stuff. Everyone probably has some opinion about how to dimension something, but there’s always some best practices to follow, particularly in a parametric design program like SolidWorks. Here’s some tips that might help.
Select an edge instead of a point
When you select an edge you’ll get a dimension right away. This goes for circles as well as lines. If you select an edge of a circle you get a radius, but if you select another edge it will pick up the centerpoint.
Dimension how you want the part to change
If you want a hole to stay one inch off the end of a part, dimension it like that.
Add relations before dimensions
This will keep your sketches cleaner and more parametric in my opinion. Like if you have a bunch of circles that need to be the same size, use an equal relation instead of dimensioning them all.
Display dimensions flat to screen
This one may be a preference, but if you work in some complicated sketches or a particular coordinate system, it may help. In Options, Display/Selection, uncheck the Display dimensions flat to screen. Play with it and see what works best for you.
Make relations and dimensions work together
To center a line, use a midpoint relation to pick up the center of the line and put a dimension on the length of the line.
Right Click to lock a dimension
If you’re working in a tight location or an angle, get the dimension in the orientation it needs to be then right click.
Link Dimensions between sketches
If you need to make sure a group of dimensions are always the same, select them (ctrl-select) then right click on them and select link values.
Drive them with Equation or Design Tables
If you really want to get fancy, you can drive some of your dimensions with Equations and Design Tables. Equation will let you make a dimension equal something. Design Tables let you make a dimension equal something for each configurations.
So, was this helpful? Do you have some dimensioning tips that help you?
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Could you explain more about “to center a line”? (under Make relations and dimensions work together)
Best Regards,
Hung Le
Yeah sure. Say you have a line that you would like centered on a point. Select the line, then the point and give them a Midpoint relation. Then, with the dimension tool, select the line and locate the dimension. When you change the dimension, it will stay centered on that point.
You can also do this with the Symetric relationship. If you have a construction line (centerline) and two other entities, like circles on each side of the construction line. IF you select all three, a Symetric relation will show up in the property manager to the left. This is one of the most useful relations by far.
Let me know if that answers your question!
midpoint is great for rectangles, many times the first sketch of any part starts with a square, or rectangle. Draw your rectangle anywhere, then draw a construction line diagonally from corner to corner. Select the origin, hld ctrl and select the construction line, then tell click on the midpoint button to make that relation (or set up your sketch constraints to your num-pad like I do, 5 is midpoint)
Now your base sketch is centered in both x and y directions. Makes things much easier when you have to change the size of your part and still keep other features relative
Right on Kyle. that is a handy little trick. guess what too, in SW 2008 there’s a centered rectangle command. After all these years!!
I was watching the new videos on SW ‘08 and that centered rectangle tool looks like it will make things even easier. On another note, I started using cross-part equations as an experiment on some of my parts. One thing I’ve noticed about referencing other parts or assemblies is sometimes the equations fail and can’t find a solution. Before you go and delete all your hard work, check and see if the referenced part is loaded lightweight. And if it is still set to resolved, edit the part in place and just give it a quick rebuild. That usually gives SW a chance to figure out what’s going on.
Hi Steve, the centered rectangle tool is definitely a much need addition. On the equation part, you may be using a driven dimension in your equation that is causing you to have to rebuild twice or open and rebuild. An example of this would be if you had a pattern instance based on the length of something. You can try to do this through just using relations and the geometry, but sometimes, depending on the situation, it can not be avoided.
Hey my company is going from Solidworks 2007 to 2008 and we are having some issues. The auto dimension feature is placing ordinate zeros wherever it wants… Not where you want to place them. Any help would be nice. Also is there a way to get a autodim button on the tool bars? still havent figured that out either… thank you
HI Tim, I’m running SP 2.0 EV and am not having problems locating the ordinate. what SP are you on? The command for the auto-dim, is called Fully Define Sketch and is located in the Dimension/Relations section on the toolbars. You can get the button from there.
I know about the fully define sketch when working on the part. Im talking when making a drawing of the part. Thanks though… As far as the service pack we are runnning the early verion currently… (1.1) So I dont really know… The one thing I do kow is i like this program more the UG i hate it lol
Hey Tim, sorry, misunderstood there. I checked out AutoDimension and it worked fine on everything I had. There’s no toolbar command for it though. I imagine that’s because it’s part of the Dimension command. The closest you’ll get is setting up a keyboard shortcut for a Smart Dimension and then switching to the autodimension tab. sounds like an enhancement request.
Ahhh To tell you the truth I never really thought of that… Thank you for the help!!!