Smart Dimensions in Parameter Table

[Eds]

Is there a way for smart dimensions to show up in parameter tables, or is it not a recommended method?

Coming from a 2D only background, I'm just starting to learn to use parameters in IC. Basically I'm trying to make a flange with parameters to drive the bolt hole circle diameter. It doesn't show up in the parameter tables, probably because it is not associated with a part/feature?

[Josh]

Right click on the SmartDimension and click "Lock" and it will appear in the Parameter table.

Note, on the image you provided this may not be possible because you are at the Part Level which means that dimension is not "Controlling" the position of the whole, it is really just a measurement. If you want to control the position of the hole, first select down to the shape (yellow) level, and then apply the SmartDimension at that level.

About 3 minutes into this video I discuss how this works: https://www.ironcad.academy/tutorial/smart-dimension#annotation

[Jonas@Solidmakarna]

For fully predictable table controlled parts or assemblies, it doesn't have to be a problem do control them by numbers in a parameter table. Maybe even the opposite. But I would never do that myself on general mech parts that are made in a milling machine or general bent sheet metal parts in an assembly. Parameters are too much work and you don't even know if the rules will apply later when you or your customer finds that you must make some late and unexpected changes, whatever reason.

Make sure to select the feature you want to "drive" first. The first " click" of the Smart Dimension must be somewhere on that feature (or whatever object that is selected). Btw, if you hold down the [Ctrl] key when left click, the Smart Dim will snap to the Anchor Point of the selected object, which is sometimes useful. You can then control the position of the object without necessarily "being" on the object itself. Holes usually (recommended) have the Anchor Point on the center point of the sketch location.

Then, the Smart Dimension must be locked = act as a constraint.

If you make the Circular Hole Pattern using the TriBall (not as rotated Linked Copies) or by using the Feature Pattern command, it will also show up in the Parameter Table. Then you can control the Angle between and Number of holes.

[Nickul]

I've done a parametric weld neck flange driven from excel and using parameters, if you want to have a look and glean any further insights.

its on GrabCAD;

https://grabcad.com/library/parametric-weld-neck-flange-1

 

Nick