toggle drawing dimension reference / driving

[creuz]

Hi, would there be a way to quickly change (toggle) a drawing dimension from driving to reference (and back)?

Does anyone have a macro or a hidden command?

Thanks

Rick

[MartinHanak]

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@creuz wrote:

Hi, would there be a way to quickly change (toggle) a drawing dimension from driving to reference (and back)?

Does anyone have a macro or a hidden command?

Thanks

Rick

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Hi,

I don't think you can do that "switching".

[KenFarley]

It would seem you are referring to the two different types of dimensions on a drawing, those from the model and those created in the drawing. You can't "switch" their types because that makes absolutely no sense. The dimensions in the model are "driving" the geometric definition of the part/assembly. The dimensions created in the drawing have absolutely no bearing on the actual geometry of the part. They are just a measure of the existing geometry that you show in the drawing.

Reference dimensions, as created in the sketches defining the geometry of the part, are measures of geometry within the sketch that might be of interest or could be used in relations. They are shown in sketches with parentheses around their values and if you attempt to change them you are warned that it's a futile effort.

[rreifsnyder]

You're correct that the types cannot be switched but there is another type within those created in the drawing. When you create a dimension in the drawing the dimension can be stored in the drawing or in the part/assembly. This is controlled by a config.pro option, create_drawing_dims_only yes/no. If it is set to yes then you are creating what's called Drafted dimensions stored with the .drw and if set to no then they are Driven dimensions stored with the .prt/.asm. The difference becomes important because you also have a choice when creating GD&T in the drawing with the same option for where they are stored. GD&T stored with the part can ONLY be attached to dimensions also stored with the part and the same applies to those stored with the drawing. 

[KenFarley]

I know about that option, but didn't want to make things more complicated than necessary. I was thinking that "driving" dimensions are the same as what we used to call "shown" dimensions. These are the dimensions that govern the actual geometry of the part/assembly, not something created in the drawing. Oh well.

[creuz]

Thanks for sharing.

[Tdaugherty]

Hi, 

Assuming this is only for drawing dimensions and you're good with parenthesized reference dimensions, here are a few mapkeys you could try.

mapkey ref @MAPKEY_LABELCREATE REF ANNOTATION;\
mapkey(continued) ~ Command `ProCmdEditProperties` ;\
mapkey(continued) ~ Select `mod_dim_new_asynch` `tab_main`1 `lay_display`;\
mapkey(continued) ~ FocusIn `mod_dim_new_asynch` `txt_dim_text`;\
mapkey(continued) ~ Update `mod_dim_new_asynch` `txt_dim_text` `(@D)`;\
mapkey(continued) ~ FocusOut `mod_dim_new_asynch` `txt_dim_text`;\
mapkey(continued) ~ Activate `mod_dim_new_asynch` `psh_ok`;

mapkey nref @MAPKEY_LABELCREATE REF ANNOTATION;\
mapkey(continued) ~ Command `ProCmdEditProperties` ;\
mapkey(continued) ~ Select `mod_dim_new_asynch` `tab_main`1 `lay_display`;\
mapkey(continued) ~ FocusIn `mod_dim_new_asynch` `txt_dim_text`;\
mapkey(continued) ~ Update `mod_dim_new_asynch` `txt_dim_text` `@D`;\
mapkey(continued) ~ FocusOut `mod_dim_new_asynch` `txt_dim_text`;\
mapkey(continued) ~ Activate `mod_dim_new_asynch` `psh_ok`;

Since the mapkeys add or subtract characters from the prefix and suffix of the dimension, it's hard to make mapkey that would toggle. You may need to investigate more elegant solutions.

Ty

[creuz]

Thanks Garnet, that's a start.

To clarify, I am only talking about dimensions placed in the drawing. When I said driving, I meant from a design standpoint.

[creuz]

The reason this came to mind is Creo is doing nothing special with the reference dimension command, just adding parenthesis to the dimension text box. So I figured a switch should be easy to make.