Adding Cut Depth to Drawing Dimension

[VELCROW]

Is there a way to have the extruded cut depth be included in the cut dimension on the drawing, just like it is done with a hole-wizard hole? I know in Pro/E you can switch dimensions to find the name of the dimension, and then just include it in the drawing dimension text in <> or something.

Thanks,

Steve

 

[CorBlimeyLimey]

Use the Insert > Model Items function.

 

[VELCROW]

I tried that, but only the in-plane dimensions come up. I'm using 2009 SP3.

 

[CorBlimeyLimey]

Not too sure what you are trying to accomplish. Can you post an image or sketch?

 

[GIDS]

If the question is how to have dimensions from your model show up in your drawing sheets, when you insert the appropriate drawing view into the sheet from the insert>drawing view>model view options be sure to select import annotations and design annotations from the import options section. You might also need to include items from hidden features.

If that doesn't do the job, go to insert>model items and select the view. Choose entire model from the source option and select the appropriate dimensions to include. This should import the needed dimensions. You can hide unnecessary dimensions.

If you want to show the dimension for a cut extrude feature in your actual model drawing simply double click the feature and the dimensions will show.

hope that helps

GIDS
Gill Incorporated Design Solutions
Reliable Solutions By Design

http://designsolutions.gillincorporated.org

 

[mncad]

I believe Velcrow wants to add a dimension to a dimension... lets say he has a slot showing the width, he would like to add the depth to the width dimension getting something like 1.000" WIDE X 1.000" DEEP. Unless the capability has been added to SW2009 I don't believe you can do that. You can add existing dimensions to notes, but you cannot add a dimension to another dimension.

mncad

 

[VELCROW]

Sorry, I will be a little more specific. I want to create a hole using extruded cut, and have the diameter and depth show up in one dimension on the drawing, just like if I did it with hole wizard. The data is in there, I just don't know if there is a way to access it.

I tried model view as GIDS suggested, but the depth doesn't show up. The only way I can get it is to do a section view. I tried shift-dragging the dimension from the section view to the front view, but it didn't work.

I can see the name of the depth dimension, D1@Extrude2. Is there some way to put that in the dimension text of the diameter dimension?

(Yes, I know I can use hole wizard, but if the cut is irregular or slotted, I don't think I can.)

 

[GRF]

Have you tried to use the hole call out tool on the annotation tool bar. Or Insert\annotations\hole call out. This will work for a hole, if you used the slot command (in the solid) it will only give you the height and width of the slot not the depth. If you manually draw a slot (2 circles with two tangent lines) it gets all confused and gives you bogus info.

 

[GRF]

That should say a circular hole not just a hole. I did not try a different shape other than a circle.

 

[erock]

Was this issue ever resolved? I am having a similar problem with SW 2007. The depth of the hole is showing up as text in the drawing. I would also like the tolerance of the depth to show up. Any help would be greatly appreciated. (see attachment)

 

[mncad]

erock,

Highlight the dimension so the property manager for that dimension comes up. At the top of the property dimension is the "Callout value" box, change that dimension of the hole that you want to set the tolerance for, then set the tolerance. You must do this before changing any of the text in the dimension text box, if you change the text at all then the "callout value" box goes away, or at least it does in my SW2007 version of SW.

mncad

 

[erock]

Thanks for the response mncad.

I should have been a little more clear about my intent. What I am trying to do is make a design library feature with a spot face and a 4 bolt pattern around it. This feature will be dropped into an existing part on top of an existing hole. I will add size and tolerance to the design library feature. The idea is, when the person detailing that part uses the hole callout feature they won't have to add the tolerance.

The problem I was running into was that when I use the simple hole in hole wizard or cut extrude, to make the spot face, the tolerance for the depth comes in as text and the tolerance does not show up.

I did find a work around. When you use the regular hole function of hole wizard and say you want the end condition to be "blind", you can then give it a depth and manually change the "angle at bottom" to be 180 deg. Once you exit from the hole wizard, you can then change the spot face diameter and apply tolerances to that and the depth. This seems to work and imports all dimensions as parametric in the drawing when using the hole callout function.

Sorry for the long winded response. This was my solution, as always there are multiple ways to do things in SW.