Why is it that a simple parts like an O-ring can't be detailed in Solidworks without having to resort to splitting the surfaces?
I create a simple O-ring with a revolve and it won't let me pick any of the edges in the drawing. What am I missing? It's such a pain to have to go through anything round splitting edges so you can detail. Then you have to go though the drawing and high all the unwanted split edges that end up showing up in other drawing views. It Sucks!!!
Use a section view in your drawing instead of adding an unnecessary split line to your part.
make sure sketches in your drawing are set to visible & then show the sketch from the feature that you wish to dimension & to some vertex or arc in your sketch at the drawing & then hide that dimension after your done.
Hope that helps Steve T.
I agree with you. There are always work arounds but you would think that such a simple thing would be possible. Every year we get a new releases with even more ways to do the same things but the basics are often ignored. Rant over! Roger
Guy's thanks for the idea's. I do use these workarounds already and have some others like copying and pasting a drawing views make the edges become selectable. Sometimes though none of these seem to work or be a good choice.
I guess I was just hoping I was missing something rather basic.
Doesn't it just seem like this is such a very basic function in a CAD package? Shouldn't this just "work" in a Super-duper high-tech, program like this? These are the kinds of things I wish they would fix before adding any more bells.
Last I worked on UG (c. 1999) and Pro/E (c. 2001), the same issues were apparent when detailing O-rings. Pro/E usually wasn't as big a problem as we usually used the model dimensions.
Maybe that's another possibility: insert model dimensions into the drawing.
Or show the sketch used in the revolve to create the oring and dimension that.
I doubt abc needs the work arounds, its the lack of basic functionality that's the point here.
I think "lack of basic functionality" is a bit harsh. I noted challenges with detailing O-rings on different CAD systems.
Try to imagine what the program is trying to do. An o-ring is a single toroidal surface. No breaks, flats, or edges. Every silhouette actually wraps around the entire part, making the logic for selection and attachment of dimensions inherently ambiguous. Computers hate that.
When working with 3d modeling programs, detailing often needs these workarounds. It's the same in any cad package. I often have to show sketches for detailing purposes in UG. Some programs do a little better but none will detail like Acad cause in Acad it's not real. You are simply drawing a circe to make the o-ring and thus it dimensions fine.
This is one of the benefits that Solid Edge has over other modelers in drafting. It creates associative lines/arcs/circles/splines in the draft file, so you get the best of both worlds... 2D data like ACAD and model associativity. Your dreaded "o-ring" is apiece of cake to dimension in Solid Edge.
Catia V4 created views that way as well (Not sure about V5).
Problem there was large assemblies took hours to rebuild all the drawing views. The upside was you modify the lines and arcs like Autocad, though a rebuild would undo it.
That's one reason we switched to Solidworks from Catia. I benchmarked a moderate size assembly. Catia took 15 minutes to update just 3 drawings views. Solidworks took maybe 15 seconds.
No need to pick sihouette edges .
When creating the part model, place the dimensions approx where you would like to see them in the drawing. In the drawing use insert "Model Items - Dimensions" selecting the "use dimension placement in sketch" option. It may look a mess at first but it does not take long to sort out what is needed/not needed, I find it best to dimension one view at a time using this method.
Why manually input a dimension when it is already there? less chance of missing one or picking the wrong edge/point and you get the funtionality to change the model from the drawing.
Just my two pence worth.
Brian
That is one thing I missed in SE. You had to tell it to fix the drawing. When it did it marked any changed dimensions with a REV symbol. I didn't always want that. But it did help in recognizing what changed. SE also didn't always bring in all the dimensions.
Ken is right though. SE drawings can stand on their own and can be opened without the model.
Well if you save drawings in the "detached" format, you can open them without the model. Of course the file size blooms when you do that due to it storing all the edge info.
How large aer Solidedge drawing files in comparison?
You would need to find a parasolid file and put it into both, same set of views, same set of line rules (visible/hidden/tangent on/off) and see. Find me a model and set the views and linetypes needed and I'll get you a number.
Ken, I would also be interested in that figure. That was a feature that I liked when I saw a SE demo, but I also wondered how big the filesize would be. Can you take a parasolid from McMaster or another site to try this out?
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