Dimension a circle in section view

For years I've tried to figure this out, but haven't the slightest idea if it is possible. If it is possible, how is it done?

See

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Currently I use multi-jog leader overlaid on itself to look like two arrowheads. It's certainly not the cleanest solution in town and rather difficult to get lined up.

Any ideas?

Any clever alternatives?

Thanks,

Reply to
cdubea
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Perhaps a horizontal break in the view, add dimensions, then crop out the top half?

It has yet to fail me (= "I haven't actually tried")

Reply to
That70sTick

Tried it. It has failed me.

Reply to
That70sTick

LOL!

Thanks I needed a good laugh. =========================================================================== Chris

Reply to
Chris Dubea

What I've done in the past is draw a construction line at the center in the section view. Then I convert the edges that want to dimension. Dimension these edges from the construction line; position the dimension above the construction line to get the diameter dimension.

Drt

Reply to
drt

Not sure if this is what you want, but this is how I do it.... Create the detail view, but make the controlling circle big such that both sides of the diameter can be seen in the detail view. Insert diameter dimensions. The reduce the circle size such that the detail now appears how you want it to, Rearrange dimensions to look pretty.

Reply to
George

So I tried to post this twice but it never came through so here is my final try...

You can do what you are wanting, search the help file for Foreshortened Diameter for instructions. So far I have been unable to find a way to add a double arrowhead to a dimension without that dimension being a foreshortened diameter.

I would like to see solidworks add a double arrowhead to the list of arrow heads that are presented when the user rmb on a dimension arrow head. Doing that would allow the user to add a double arrowhead to any dimension.

Sam

Reply to
Sam

I would like to add that the Foreshortened Dimension only seems to work if you have an Extrude. I went round and round with my VAR to find out how to do this and we discovered it doesn't work on Revolved Cuts. Keep it in mind. I'd like to see the double arrowhead added by Solidworks also.

Jeff

Reply to
Jeff Zim

create the DIA. dimensions in an unbroken view first. Then create your detail view just like you show in the picture. Then just select the DIA. dimension and HOLD DOWN the SHIFT key and drag and drop into the detail view. You should see the DIA. dimension foreshortened. The display option with double arrows can be controlled by your tools "options" in document properties.

Don

Reply to
dvanzile3

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