Hello, I have a sketch with a lot of lines and symbols in it, when I try to fully define the sketch I currently have to pull on lines and points to see if they are under defined as the whole sketch is black.
Is there any way to see what is still under defined, I know there is a "degrees of freedom" option in Inventor so I was hoping something similar exists in SW, I don't want to use the auto define option because I want to be in control of things.
I have the different colors option on, but my sketch is all black and I have to manually pull lines and or points to find out which part is still under defined.
There is a tool for this. tools pulldown menu, sketch tools, check sketch for feature. You can also rmb click in the user interface and choose fully define sketch. More than likely you are missing a relation if you have all your dimensions pulled.
If all your sketch entities are black thent the sketch should be fully defined. Also look in the bottom right hand corner of SW and it should say either "Fully Defined" or "Under Defined.
K.,
There are a few special cases where a sketch will be all black but not fully defined. Offset Entities are one, where the end points of an offset entity show up black, but you can still drag them. I can't remember the others.
Come to think of it, the sketch may say that it is fully defined in the case of the offset entities, even though it still has some freedom left.
Jerry S.
'Converted' entities (edges) are the most-common sketch entity whose end points can be 'pulled' even though they're black. This is something that is both very useful and very annoying depending on what you're trying to achieve on the day! Sorry not to be able to help in a more-positive way.
Keith
Try toggling 'Color Display Mode' (line format toolbar). By default, SolidWorks should show you if goemetry is fully defined or not using a color coding system that's visible while editing the sketch. HOwever, if you want to display arbitrary sketch colors, you can toggle this off (which is useful for drawings where you want to display sketch symbology instead of status). So your may have been turned off at some point.
Once you've exited the sketch a '-' preceeding the feature name indicates that it's underdefined (a + means it's over defined and no symbol means it's fully defined)
As K. Hampton said, "under defined", "fully defined" or "Invalid" will appear in the status bar at the bottom right while you're editing a sketch.
Finally, if you have 'Override dims on drag/move" enabled (Tools>Sketch Settings), then you can drag points constrained by dimensions and the dimensions will change. So your efforts at testing a sketch may actually be changing it in that case.
Check those out and let us know.
John
Look very closely at the endpoints of all of your lines. A line can be black, while the endpoint is still blue. This indicates that the endpoint can only move back and forth along the line.
Another thing that can cause problems are two lines stacked on top of one another. The shorter line will not be visible at all. Also, very short line segments that hide near the endpoints. (I see these problems often in the introductory class that I teach)
You want to try and keep each individual sketch as simple as possible. It makes it much easier to find problems. Rather that try to create the entire profile of a part in one sketch, start with a simple block/revolve, then add or remove material a little at a time until you get the shape you need.
I have found the little bugger, it was a line on top of another line. I will try making sketches simpler, I used to make one big steering sketch with all features derived from it ( this worked perfectly in Inventor). Anyway, thank you for the responses and tips.
The simplest way is to have seperate colors. The default setting for sketch entity colors is black for fully defined and blue for under-defined. If that's been changed, you can set it to whatever colors you want at Tools > Options > System Options > Colors > Color scheme settings.