How can I put linear dimensions to centerlines located off the drawing page?
Running 2010 here but the preview image gave me enough to try what I think you're trying to do. I don't recall ever seeing this before, but then I don't think I've tried doing this before. I would probably have just added a scaled down view with the 1:1. Anyway, I dimensioned the two end points to the inside arc, not a center point off the page. Then, when I foreshortened the radius dimension the horizontal and vertical dims went along for the ride. I tried it twice, whichever radius you foreshorten first is the one the horizontal and vertical dims latch onto. Maybe not what you want, but interesting enough that I thought I'd throw it out there before lunch break is over, just to see if anyone else has anything to add about it. I think I got the part and drawing attached, in case anyone wants to play with it.
Good morning Raymond,
Back in 2004 you could select a drawing view and stretch the drawing view to add a line or circle etc.. Now it is a little different and hopefully I can explain it here, if it doesn't make sense let me know.
Now you can draw a centerline/construction line with in the drawing view block and add a dimension from that line to a existing centerline of the part, lets say 500" and this will stretch the view box and if that crosses over the centerlin you want then select it and if you can't select it, make sure your Selection Filter tool bar is in the Sketch Selection mode.
Just draw you centerlines using the sketch centerline in the sketch toolbar
and dimension to them.
Are you talking just in the drawing or are you looking for this to be incorporated into your model as well?
Just to the drawing. I have added my drawing and part to help clarify. I know about foreshortening the rad. dimension, its the linear dimensions thats the pain.
I see what you are tlaking about.
RC on the sheet in the feature manager and select properties.
Then go to custom sheet and enlarge the sheet.
Don't really want to enlarge the sheet if I can help it. But if thats the only way... Would like to keep the drawing 1:1. But if Solidworks will not let me forshorten the linear dimensions or be able to break them somehow, then I will do that.
Good afternoon Raymond,
Why would you be stuck with a 1:1 ratio?? (may be none of my business) but if it is for dxf or dwg exporting there are work arounds there also.
I know its not good practice and should not ever be done, but our shop guys (only on parts that are not critical in any way) will lay the part on the drawing to check the size. They only do it on parts like this that will be water-jetted only with no machine work. This particular part could be missed by .015 and still be used.
Think about it; it eliminates QC.
Understand that by enlarging the drawing sheet does not mean that the view is
not still 1:1 All you are doing is moving the borders out. The view remains the same.
Now when you go to print it out that is a whole different ball game. That will not be 1:1
I thought there was some way in Solidworks to foreshorten the linear dimensions. I guess I was mistaken. I need it printed out 1:1. ( you can read my statement above) . Then again it would be just fine to print out to a different scale so the shop would not use the drawing as a template.
The foreshortened dimensions come with broken views.
I guess you have some choices to make now that you know your limitations.
Thanks everyone for your help.
Why not place both views on the sheet temporarily and use the foreshortened dimension. Then move the unneeded view off the sheet.
There is another work around, it's not a foreshortened dimension, but it works. After adding your linear dimension, right click on the extension line you don't want and hide it. Then right click on the dimension (on the side of the dimension you don't want to see) and hide it. Then move the text as close as you want to the remaining extension line (make sure to turn off the Center Dimension under Display Options for the dimension also).
Hey that is it! Exactly what I was looking for. YOU DA MAN!. I do appreciate everyones help. Wish they tell you these easy things somewhere but guess thats why the forum is sooooo good. So just go ahead and dimension all linear dimensions you want and then foreshorten the leader. GEEEEE. Simple.
I hope you checked to make sure this actually works for you. I suspect that this is not "official" SW behavior and that someone somewhere is fixing this "bug" as I type. For instance, you will note that the radius centers don't stay coincident and additional notes would be required to clarify if this is the case or not. Also I would check that everything updates correctly when you change the model.
Until I see or hear otherwise I am treating this as potentially handy, but unofficial, and undocumented behavior. Who knows what it will do tomorrow. Definitely in the "use at your own risk" category. It is kind of cool though.
If I were doing what it sounds like you are, (and I have in the past, on occasion) I would send the guys a drawing like this. That gives them a full size view with whatever dims are needed or desired (this sort of thing was usually an informal request from someone) and then an additional view(s) with info that the laser/punch operator would need to manually develop and input a program. I.E. the location of radius centers, start and end angles etc.
Have fun, let us know how this works for you, or not.
Yes it worked for me. I am running 2011sp5. I repeated this several times throughout the day just to see how it reacts. It does react unpredictably. Sometimes it works good others it would throw one of the linear dimension way off to the left. When you try to drag it back it starts behaving oddly. The numeric value of the dimensions remains correct but the dimensions sometimes disappear or they may remain and the zigzag foreshorten symbol will disappear.
Thanks for the advice on doing the drawing a different way.
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