Can Dimensions / Smart Dimensions "drive" part size?

[Macktek]

Hello,

When creating an "Innovative Part" and creating a Smart Dimension, for example between two edges on the face of a cube, it will display the current dimension (in this case 0.050).

However, if I edit the dimension with a New Value (such as 0.1) , it goes thru the process as if it is being edited, but upon completion, nothing happens.

How can I edit the Smart Dimension to change the Part Size? Or do I need to use another dimension type to do that?

(I am aware of handles, but that's not the same as visible dimensions)

Edited June 7, 2020 by Macktek

[GNÄSLUND]

You can also try adding the dimensions in the cross section sketch. They can then be edited from the 3d scene

[Macktek]

OK so I am giving "Edit Cross Section" a try... and I am testing on a simple "Poly" from the shapes catalog in an attempt to make a Hexagon that I can adjust by simply typing in a dimension. So, I tried that but it warns me that "Any modifications to the profile will remove these variables and may yield undesirable results" (continue ?). I press yes, and continue.

Adding the dimension allows me to adjust but, it deforms it out of shape, so I need to add constraints.

I then add a set of angular and equal length constraints to the existing diagram, as well as 1 dimension across one of the faces.

But when I attempted to use it, it gives me this error: (and oddly converts it into a rectilinear cube shape in preview)

 

 

Edited June 7, 2020 by Macktek

[Malcolm Crowe]

Hi,

When it comes to sizing of standard "Intellishapes" (without the need to constrain everything in the 2D sketch), there is the option to use "Sizebox Dimensions". By default these aren't visible, but by right clicking in the scene, select "Show" and then toggle on "Sizebox Dimension". The first part of the attached video demonstrates this.

Something else that my be of interest to you is the option to show "Position Dimensions". This is demonstrated in the second part of the attached video.

Malcolm

[Macktek]

Thanks again Malcolm,

I see that option is useful. But unfortunately, I don't think it solves the general problem that I can't seem to use Smart Dimensions in the scene to drive line lengths, angles, etc... (as mentioned in another post, when I smart dimension a line segment of a part, editing the size of the smart dimension doesn't do anything.

(Perhaps there is a setting that I am not aware of, such as "Allow Smart Dimensions to Drive Part Features"?

Edited June 8, 2020 by Macktek

[Jonas@Solidmakarna]

Hi Macktek,

First, I think you should have a look at the basic training material available online. It will answer most of the questions you don't yet know that you have!
https://www.ironcad.academy/tutorial/training-01

The Smart Dimension tools that you have found are mainly used for positioning objects in 3D space. Not for manipulating/driving the size and shapes of them, just as you guessed. Btw, you can toggle the visibility of the Smart Dimensions with the glasses at the bottom:

The red handles found directly on the shapes (another click with the left mouse button after the blue edges) are the tools you are supposed to use for changing their dimensions.

So if you use the Smart Dimension tool to place a dimension between two points/sides of the same assembly/part/feature, it is "only a visual dimension". It won't do anything else (like modifying).

You can see the shapes dropped from the catalogs as schematic in one way. They are made to be modified only to keep their individual shape, where a block is a block, a cylinder is a cylinder and a polygon is a polygon (though the number of sides can be modified). The red round Sizebox handles on the Intellishape level will scale the models and still keep their "relative shape" intact.

If you want shapes that have another kind of rule or shape, you must make them yourself from start. Use the Extrude tool or edit the Cross-Section of an existing Extrude feature (Block, Cylinder or Polygon). If the shape should be defined by some kind of "rule" (like in parametric control) you must add those rules yourself. Rules are mainly defined in the Sketch/Cross-Section by Smart Dimension Constraints.

Just like in any parametric CAD system you must (probably) make the curves "fully defined" (green color on curves, instead of the blue "under-defined" color) in order to follow your expectations.

As Malcolm said, the thing with IRONCAD is that you don't really need to add constraints to get things done. Most kinds of parts are easier to manipulate using the red handles (which in turns will manipulate the blue "under-defined" sketch geometry), because it is much faster to find (snap to) values with the help of other geometry in the scene. Only when you want to edit assemblies and parts like bearing houses, steel profiles and other "table controlled" types of parts, then the need of adding rules might be useful.

[Cary OConnor]

For the Polygon, there are a couple different ways to do this. 

1. The Polygon shape in the catalogs. When you drop this out, there are two ways to really size that shape. One with the intellishape handles and the other is by right-clicking on that intellishape and selecting Intellishape properties and going to the variable tab which will allow the polygon number count and sizes in meters. 

2. Start a sketch. Under the the Rectangle Drop down, there is a polygon shape. Click that and place the first point on the sketch. In the Browser, you can change the number for the shape. Place the second point. Once you create this, it should create some default relations and you can add other dimensions to drive the shape. 

Attached is a video to help out.