Sketch constrains

[raghudvg26]

Hello everybody.<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />


Can anybody tell me how to check whether sketch is constrain or not and also check for open and closed contour in sketch mode itself.


Raghu

 

[SSLaser]

On the lower right side of the SWX window, you'll see either "Fully Defined" for a fully constrained sketch, or "Under Defined" for an under constrained sketch. Another visual cue is that fully defined sketch elements turn black, under defined elements remain blue.


The open or closed contour question can be difficult at times- occasionally, an errant mouse click will leave a little tiny line at one of the corners or line intersections. If SWX thinks there is an open or multiple contour for something I know should be closed,I right click on a line, choose Select Chain, then hit the delete key- this sometimes results in the errant line being left behind, click undo

to bring back your deletion, then delete the errant line.

 

[nucu]

Hi

Try (menu) Tools->Sketch Tools->Check Sketch for Feature.

Nucu

 

[raghudvg26]

Hi


Nucu


I tried what you said, i got clear about that things, thanks


raghu

 

[KoustubhK]

one more point


if u look at the sketch in model tree (at left hand) if it shows - (negative) sign then it is underconstrained.


if it shows+ (positive) sign then it is overconstrained.


And no sign means fully constrained

 

[sunilbadkar]

look sketch in model tree (at left hand) if it shows - (negative) sign then it is underconstrained.


if it shows+ (positive) sign withthen it is overconstrained.


the colour will indicate type of error in sketch like red -overconstrained


greenish like

this will give reference problem.


And no sign means fully constrained


If sketch is not closed the u can see the differance of


thickness in line font. Try the open sketch and closed sketeh in on


command u will know the differance.

 

[Mindripper]

Of course, a blue line or point is unconstrained or underconstrained, and a fully constrained line or point is black.


Since the endpoints of centerlines are not required to be constrained, this condition will not result in a minus sign on a regenerated sketch. But you can use the endpoints of centerlines as sketch references, and they can be constrained if you wish.


SolidWorks is also quite tolerant ofredundant constraints in many cases. But do try to avoid this, as this can make debugging sketches difficult.

 

[raghudvg26]

hey


Tahx for replying, I got it