fully defining sketches 1

[qwiteconfused]

I've just begun using solidworks 2001 after using ProE, Alias Studiotools and Autocad. After following the Solidworks tutorials (hinges, flashlights and mould tools)and modelling some objects of my own I repeatedly run into the same problem. When I get to the stage that i want to end a sketch and create a feature, i get the message box, 'this operation requires a fully defined skecth'. I took this as meaning that some of the ends of the sketch were 'loose' and needed joining up which I did. (I cannot find a snap to object command either! - this would help I feel!) SO i have several sections that I cannot continue with because the sketch isn't fully defined.

 

Go to tools, options, system options, sketch tab.... the first option on the page is use fully defined sketches. If this is checked you will be required to fully define each sketch prior to using it for a command.

 

[Troup]

Fully defined is not the same as trimmed (ie joined up) which was all you needed to worry about in 2D

In SolidWorks, ideally all sketch entities should be black. In the case of, say a rectilinear rectangle, this would require applying a "horizontal" constraint to two lines, a "vertical" to the other two, snapping (say) one corner to the origin, and dimensioning width and height.
If you don't fully define all entities, there is forever after a risk of something getting dragged out of kilter in that sketch.

 

[qwiteconfused]

is there a "snap to" function that means that all lines drawn can be snapped to other lines without the need for constant zooming in and re-addressing the lengths, diameters etc of the shapes. I have tried the command in the tools/options/grid snap but this does not seem to snap to a grid or any line object that i draw in sketch mode?

 

[MadMango]

If you move your pointing device around during sketching, you'll notice that the icon will change when you are on an end point, midpoint or other feature. This might be the "snap-to" feature you are looking for. While sketching, if you start and stop sketches according to the changed icon of your pointing device, you should have automatic constraints.

In SW, the only snap-to options are for Horizontal, Vertical and Angles (default 45).

I have to agree with Troup on fully defined sketches. Its a very good habit to use fully defined (all black) sketches in your models... and archoring your sketches to either the Origin or Planes. "The attempt and not the deed confounds us."

 

[BBJT]

You may want to turn on display entity end points under Tools Options Sketch. If this is not check you will not see the end points of your lines which may be blue. If you do see blue sketch entities left cleck and drag one and see what it does. You should be able to determine what is missing by doing this. BBJT CSWP

 

[SBaugh]

I use Auto relationships tools\options\sketch which help out in this situtation. I also use fully defined sketches...I don't have the option checked but I make it a point to fully define them.

Time to hit the hay

Regards, Scott Baugh, CSWP
credence69@REMOVEhotmail.com

http://www.3dmca.com

http://home.insightbb.com/~scott.baugh/

*When in doubt always check the help*