Need help with under defined sketches

Hello,

I'm new to Solidworks and I should mention right away that I'm not a
mechanical engineer. I do have, I'd say, about 10+ hours of experience
with Solidworks and it certainly seems like an impressive program.
I've gone through many of the tutorials but I am still having a lot of
difficulty figuring out how to fully define my sketches.

I've looked through the help files and searched this group but I'm
unable to find anything to help me get around this problem. Is there a
systematic way to determine WHY a particular sketch is undefined? I've
tried to define my under defined sketches by using the 'Smart
Dimension' tool, but to no avail.

For example, I have a simple 1/2" thick extrude into which I've placed
a hole. The sketch that makes up the hole is listed as under defined,
so I Smart dimensioned two dimensions: the x and y distance from an
edge, yet it still remains under defined. I assume that the z
coordinate is set by placing the hole on the surface of the extruded
part.

My intuition tells me that to be fully defined a sketch must have all
its degrees of freedom set, but even when I think I've done that, it is
still not fully defined. I'd really appreciate any input into this
problem.

Tim

 

Did you dimension the diameter of the hole?

 

If you can see anything that is blue, that is undefined. So, let's take
your hole, for example. If it is blue, grab it and try to move it around.
It will only move within the underdefined degrees of freedom. You mentioned
that you dimensioned the x and y distance, but did you dimension the
diameter?

 

The best way to figure it out is grab and drag what ever is blue. It
should move. The exception is if you are using splines in a sketch, I
have run into sketches with splines where everything is black and it
still tells me that the sketch is underdefined.

KM

 

as others have stated, it's the diameter which is underfined.

to further assist in diagnosing underdefined sketches,
under tools, options, system options, sketch, check the following,

display arc center points in part/assembly sketches
display entity points in part/assembly sketches

enabling these 2 options will display the infamous "invisible blue spots"
(e.g. end points) which will also lead to underfined sketches.

 

Please forgive my total ignorance. I've read about under defined parts
being blue but I'm not sure I've seen it. Should I see it in 'sketch
mode' or when the part is displayed 'normally'? If I edit the sketch
that is under defined, the hole disappears and it allows me to edit the
point that forms the center of the hole. But this still remains under
defined.

As far as grabbing and moving things, I can't seem to do it.

I created the hole using the hole wizard. Does this mean that the
diameter is automatically dimensioned?

My options already had

Display arc centerpoints in part/assembly sketches
Display entity points in part/assembly sketches

selected, yet I'm still not sure if I'm seeing anything in blue.
Thanks for the help so far.

Tim

 

I'm guessing you probably need to a dimension or locate you sketch to
either the origin or base planes

 

Back when I was first learning SWX (on 2001) I found a bug in the Hole
Wizard, I don't know if it's fixed or not but, generally you want to select
the surface you wish to place the hole on *then* click the Hole Wizard
button, otherwise it'll create a 3dSketch for the hole location. Not sure
if that's a problem anymore but it caused me a bit of a headache in the
past.

2¢
Whit

 

Timbo,

Are you using the "simple hole" or the "hole wizard"

Simple hole uses an extruded circle. You just have to dimension the X,Y
center

Hole wizard creates two sketches. The first one is just a simple point on a
face. The second one is a revolved sketch. Axis of revolution, on the second
sketch, is referencing the point on the first sketch. If you edit the first
sketch and dimension the X-Y of the point, both sketches should be fully
defined. This is because the revolved (second sketch) profile is already
fully defined except for X,Y, (which it gets from the point (first sketch).

This sounds (and is) much more complicated than it has to be, especially for
a newbie. I dont use the hole wizard much myself because it creates so much
geometry. Sometimes I really need to define the drill point, and then I'll
use it. Otherwise I just draw a circle and extrude it.

To demostrate color changes fo under/fully defined sketch elements, start a
new part. Start a new sketch and draw a rectangle, the lines are blue.
Dimension one side, still blue. Dimension the other side, still blue.
Dimension one vertical line to the origin, vertical lines turn black.
Dimension horizontal line to origin, all lines are black. The sketch is
fully defined.

On the flip side, don't think that just because all the lines are black it's
OK. Ther should always be an intentional "structure" to it. It's possible do
define a sketch so that it's fully defined, yet when ever a number changes
it goes "over defined" or "unsolved". To minimize this, don't use complex
sketches (ala-ACAD). Build your models using features.


Regards

Mark

 

It sounds like you used the hole wizard without first selecting the
face that you want the hole on. This will give you a 3D sketch point
to locate your hole. Since it is a 3D point you will need to locate it
in X,Y, and Z. One thing you can do is to edit the sketch with the
point in it and select the point and the face that you want it to be on
and add a coincident relationship. This should give SW enough
information to fully define the point.
If you select a face before hitting the hole wizard icon you won't need
to do this.

Todd

 

OK, this is really helping. Thanks. My part has three holes, one has
been dimensioned to the edges of the part, fixing it in x-y and it is
fully defined. One of the other two holes has its x dimension
dimensioned to the edge of the part and the y dimension is dimensioned
to the center of the first hole, but it us under defined.

Shouldn't I be able to define a sketch with respect to another, fully
defined sketch?

Tim

 

Without seeing your sketch, you may have dimensioned from a quadrant of the
circle instead of the center of the circle. If this is the case, it will
take more dimensions to fully lock it down. Make sure your dimensions are
going to the center of the circles instead of to somewhere on the
perimeter.

 

Tim,

You can only drag sketches while you are in (editing) them. Select any
line/arc etc.. and hold down the left mouse button, and drag it around.
This helps you SEE what is going on better thatn any other method as you
can SEE which dimensions are constraining and which are not. Also, the
sketches in hole wizards are a lot more difficult to debug, when things
aren't working the way you want. Unless you really need the benefits of
hole wizards, I would stick to regular sketched features, until you get
more familiar with constraints. Constraints take a while to anticipate
and understand, and is where most of the learning curve is steep. But
learning to drag stuff around helps tremendously in getting past that
hump. Also, So called Smart features aren't always as smart as you think
they might be, or want them to be.

ca