sketcher known dim in Creo 2

[davehaigh]

How do you create a known dim in Creo 2.0?

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550

[mlocascio]

David,



Are you referring to the idea of looking up (or showing) the dimension ID so
that you can use it in a created dimension?



Mike Locascio

[davehaigh]

If you switch dims in the sketcher it supposed to have the symbol kd#

You can then use it in a sketcher relation

David Haigh

[mlocascio]

That's the idea. BUT it's NOT a "kd#" - it should be an "sd#"



MPL

[davehaigh]

From the help:
sketcher_known_dim_on_ref_entity
yes*, no
Controls the type of dimension created for normal dimensions with only background geometry selected as references.
yes-Creates known dimensions, for example kd#.
no-Creates reference dimensions, for example, ref#.

But I just want to create it not set a config to create it.
Known dim's have been in ProE since the single digit revs of the software.

David Haigh

[davehaigh]

From Wildfire 4 help topic collection. How do I create one of these in Creo?

About Known Dimensions
A known dimension is a dimension for a single reference entity or between two
reference entities. A known dimension is represented by the dimension symbol prefix
kd#. In the Sketcher mode, you can use the references and known dimensions to
create a relation.
To Create Known Dimension
1. Click Dimension on the Sketcher toolbar. Alternatively, click Dimension on the
shortcut menu.
2. Select two edges, two vertices, or datum entities.
3. Middle-click at the required location to place the known dimension.
To Create Known Dimension (OFF)
1. Ensure that the Intent Manager is OFF on the Sketch menu.
2. Click Sketch > Dimension. The DIMENSION menu appears.
3. Click Known.
4. Select two edges, two vertices, or datum entities.
5. Middle-click at the required location to place the known dimension.
To Use Known Dimensions (OFF)
Known dimensions allow you to establish meaningful parametric dependencies when
creating a section of a feature.
1. Ensure that the Intent Manager is OFF on the Sketch menu.
2. Sketch and dimension as usual.
3. Create Known dimensions on part geometry that will be used to drive the
feature section.
4. From the Sketch menu, select Relation.
5. Add relations connecting Normal section dimensions with the Known ones.
6. When the system updates the section, values of normal dimensions change
according to the relations.
Dimensions driven by Sketcher relations cannot be modified directly. To access
Sketcher relations, choose Redefine and Section. You can also do it in Part mode
by choosing Relations, Feat Rel, selecting the feature, and choosing Section.

David Haigh

[dmartin]

In general, you want to avoid Relations in sketches (aside from Variable Section Sweeps).

But if you are writing a Relation in Sketcher, you can use Known Dimensions in them. A Known Dimension is simply a dimension that you create in Sketcher on model geometry, not on sketch geometry like lines, arcs, circles, and splines.

For example, create a block and then create a sketch on one of the block's surfaces. When you go into Sketcer, before creating any entities, create a dimension from one side of the block to the other. That is a Known Dimension.

I avoid Relations in sketches because I've seen them give permanent yellow regen status, and they are very hard to detect unless you search for them deliberately. About the only ways I know to find them are to Edit Definition of a sketch and then go to Tools > Relations, or in Part Mode open the Relations dialog box, change the Look In filter to Feature or Section, and select a sketch.

David R. Martin II

Senior CAD Application Specialist

Amazon