Sanity Check: Can dangling diameter or radius dimensions be reattached?

[bnemec]

Do people just delete dimensions or try to reattach them? Seems like linear dims can reattach, but diameter or radial cannot?

Edit: looks like I struggle with reattaching linear line to line or point to line dims as well.

Thank you.

[AlexLachance]

Yes they can be reattached sometimes. Linear dimensions can be reattached when both references aren't lost. If both are lost, sometimes you can reattach them using endpoints rather then edges or faces.

[SPerman]

My success rate with re-attaching is extremely low, so I don't even try anymore. Delete and recreate is my advice.

[AlexLachance]

My success rate with re-attaching is extremely low, so I don't even try anymore. Delete and recreate is my advice.

That's pretty much it. I try to reattach in part sketches, but in drawings, to hell with that, I delete em and recreate em most of the time because there is no benefit from either.

[bnemec]

That's pretty much it. I try to reattach in part sketches, but in drawings, to hell with that, I delete em and recreate em most of the time because there is no benefit from either.

For those trying out Solid Edge. Try out holding the ALT key while click and drag the endpoint of a dimension leader then drag to a new sketch element and let go. Annotations don't need to be dangling to reassign them. IIRC it works in the sketch and drawing environment. Used to use it all the time. Seems like Alt key does nothing when working with dims or annotations in SW?

[AlexLachance]

For those trying out Solid Edge. Try out holding the ALT key while click and drag the endpoint of a dimension leader then drag to a new sketch element and let go. Annotations don't need to be dangling to reassign them. IIRC it works in the sketch and drawing environment. Used to use it all the time. Seems like Alt key does nothing when working with dims or annotations in SW?

They aren't buttons to bring up different quick commands for sketches, though they do work for the assembly environment, when mating, rotating and what not.

Tab hides parts that you're hovering over
Shift allows multi-selection, and facilitates selecting something that's transparent.
Shift +pressing wheel can be used for zoom ins/out, I sometimes use in for specific cases.
CTRL and pressing wheel will allow panning

few from the top of my head

Edit: Shift in sketch will work when doing diameter dimensions or mirror dimensions

[Glenn Schroeder]

I usually try to attach them . . . once. If it works, great, if not I delete the dimension and add a new one.

[DanPihlaja]

The answer is......sometimes.

The other answer is....since it is hard to predict when "sometimes" equates to "true", it is just easier to delete the damned thing and replace it.

[zwei]

I never like re-attaching dimension in SOLIDWORKS.... 80% of the time i cant get it to work...

Ironically, i am always able to reattach dim in CREO...


If only SOLIDWORKS has something like "EDIT ATTACHMENT" like CREO (Never thought i will say this one day...)
http://support.ptc.com/help/creo/creo_p ... rence.html

[jcapriotti]

Delete and recreate is my advice.

Slight edit "Recreate and delete".....that way you can use the format painter to copy over the dimensions settings if needed before deleting the lost dimensions.

[JSculley]

A few things I've discovered about this:

1. Imported dimensions are less likely to go dangling. This makes sense, since the dimensions are often tied to model sketch geometry which isn't affected by later features. For example, here's a drawing with imported dimensions:

If I add features that remove/alter edges, nothing goes dangling:

Of course, you can't attach the radius and diameter dimensions to the new edges. You have to delete and import the dims for the new features or add manual dimensions.

If I do the same experiment with a manually dimensioned drawing, everything goes dangling:

This depends somewhat on how the manual dimensions were created. For example, the 5.00 dimension can be created 3 different ways:

a. Select the single horizontal edge
b. Select the two vertical edges
c. Select the two vertices

Selecting the vertices leads to the 5.00 and 3.00 dimensions dangling as shown in my image. Selecting edges will lead to non-dangling dimensions, but you might end up with something like this:

2. If you have a dangling linear dimension where both references have been lost, click/drag the first witness line to reattach it. It may seem like nothing happened, but if you immediately click/drag the second witness line to reattach, it will succeed.

3. For diameter/radius dimensions, using Display Options....Display as Linear allows you to reattach. For radius dimensions, you will have to first use Display Options....Display as Diameter.

[berg_lauritz]

A few things I've discovered about this:

1. Imported dimensions are less likely to go dangling. This makes sense, since the dimensions are often tied to model sketch geometry which isn't affected by later features. For example, here's a drawing with imported dimensions:

I REALLY wish that this would be better to use. keeping everybody on the same page with this is almost impossible - that's why we don't use them... sadly.

[jcapriotti]

I REALLY wish that this would be better to use. keeping everybody on the same page with this is almost impossible - that's why we don't use them... sadly.

Design intent dimensions rarely match drawing requirements anyway which are more geared for manufacturing and tolerance considerations.

[bnemec]

Slight edit "Recreate and delete".....that way you can use the format painter to copy over the dimensions settings if needed before deleting the lost dimensions.

I try to mark my threads answred, this one is tough to choose which one, most are good. Selected this one as it has proven to be a good addition to a good answer.

[jcapriotti]

Correct answer is to submit an SPR and bug the hell out of SolidWorks.....not that works.

[bnemec]

Correct answer is to submit an SPR and bug the hell out of SolidWorks.....not that works.

pun intended?

[jcapriotti]

pun intended?

No...lol