AnsweredAssumed Answered

Fully defined

Question asked by Bjenk 8100 Jenkins on Oct 25, 2013
Latest reply on Oct 28, 2013 by Lenny Bucholz

Like • Show 0 Likes0
Comment • 9

Hello,

I recently asked and was advised to check the box that mandates a fully defined sketch before rebuild or addition of a feature. I am fine with this and like having a fully defined sketch. However, I am getting very frustrated. All I try to do is draw a simple sketch and put in smart dimensions and craziness happens (overriding sketch, over defining, etc.). What I do is go to every yellow entity (conflicted) or blue (under-defined) and select it. I edit the line properties (relations > hor, vert, fix) and then the line is defined. What does fix do. The whole thing just doesnt make sense to me. I have to go to properties and hit fix. None of the properties change from what I wanted. Solidworks attempt to explain the fully define process is not enough. Any help with something I am missing or where to go to search this concept is greatly appreciated. Drawing a fully defined trapezoid should not be a hard thing or time consuming thing to do. I have been drafting a long time with other programs and never had such problems.

THanks,

Brian

No one else has this question

Outcomes

9 Replies

Glenn Schroeder Oct 25, 2013 10:13 PM
Mark Correct
Correct Answer
I'll try to help. First of all, I understand that you've used other programs without these problems. When learning SolidWorks I had what I believe was the advantage of no previous CAD or 3d modeling experience, so I didn't have any habits to un-learn. With that being said, a fully defined trapezoid is very simple to sketch without problems. It's just a matter of learning how this software works. I didn't get a lot of specifics from your post, but I suspect that what may be causing some of the problems is un-intended automatic relations. If you agree, you might try holding down Ctrl while placing sketch entities, since this disables automatic relations, and see if that will help.

By the way, you mentioned the "Fix" relation. It just locks a sketch, making it sort-of fully defined. I almost never use this. Only occasionally if I'm tracing a sketch picture to lock sketched entities so I don't move them un-intentionally.

Another thing you might check is at Tools > Options > System Options > Sketch > Over-defining dimensions, select "Set driven by default". (See this discussion for a screenshot: https://forum.solidworks.com/message/388388#388388.) That setting will set extra dimensions as driven, preventing them from causing a sketch to be over-defined. As discussed in that post, it occasionally un-checks itself for some people, so you might keep an eye on it.

Anyway, to sum up this rambling post, try to be patient and learn how the software works and work with it, instead of fighting it and getting frustrated because it doesn't work the way you think it should. And if you have any specific situations you would like help with please post them, preferably along with the actual file that's causing you problems. Traffic is generally slower here on the weekends, but I'm sure someone will be glad to help.

Good luck
Glenn
Like • Show 0 Likes0
Actions
Erik Bilello Oct 26, 2013 12:16 AM
Mark Correct
Correct Answer
Unlike Glenn I learned ProE in school before taking SW, but at the time that may have been an advantage because the ProE instructor was a stickler and (at the time anyway) ProE was much more particular about needing things defined than SW, as I recall you couldn't even exit the sketch until everything was properly defined.

Like Glenn I will advise to avoid Fix (it's fix as in "fixed position", not "repair") as much as possible. About the only times I use Fix are with splines and in explode line sketches, which are usually more a matter of what "looks about right" than exact size or location.

The bugaboo of unwanted automatic relations will get better with experience. As you get to know what's going on behind the scenes they can become an advantage instead of a hindrance. Keep an eye on the pointer as you sketch and note what relations are being automatically added. I try and delete the ones I know I don't want, and add the ones I do as I go.

Keep things simple. I don't know where they're handing out the awards for fewest features in a model, but I've never gotten one. Making an extrude, and then adding a cut to refine the shape is often just as easy as making an overly complicated extrude sketch just to avoid adding a cut feature. My rule is that if I can't easily remember how each element in a sketch is related to the rest, my sketch is getting too complex. I have a boss to make my life complicated, and that's one area where I try not to help him.
Like • Show 0 Likes0
Actions
- Bjenk 8100 Jenkins @ Erik Bilello on Oct 26, 2013 1:39 AM
  Mark Correct
  Correct Answer
  o;seems like its all about dimensioning off of origin or somehting that has been dimensioned off origin.
  Like • Show 0 Likes0
  Actions
  - Glenn Schroeder @ Bjenk 8100 Jenkins on Oct 27, 2013 9:17 AM
    Mark Correct
    Correct Answer
    Yes, that's one basic rule that gets by some people when learning. A sketch isn't fully defined until it's position is defined in relation to the origin.
    Like • Show 0 Likes0
    Actions
    - Bjenk 8100 Jenkins @ Glenn Schroeder on Oct 27, 2013 1:53 PM
      Mark Correct
      Correct Answer
      Ok I am getting better at the fully defined stuff to a point. What you think about tools>fully define sketch option. My strategy right now is figure out where I want my origin to be before I start. Start my sketch>add dims. Usually its defined. If not, I hit fully define sketch option to see what it adds. THis actually helps me know what the program expects. The only thing it really adds is how far away from origin something is. Here is a question that would help me out. THere a way to add same feature to more than one entity. For example, if you have five circles all with the same diam. is there a way to define them all at once like the way fully define sketch option does, lol?
      Like • Show 0 Likes0
      Actions
      - J. Mather @ Bjenk 8100 Jenkins on Oct 27, 2013 2:00 PM
        Mark Correct
        Correct Answer
        Ctrl select or window select or crossing window select all the circles and hit =.
        
        I recommend that you define the relations (other than the automatically vertical, horizontal, perpendicular and tangents) rather than "what the program expects." It should be what you as the designer expects. You define the geometry.
        
        I recommend that you attach one of your files here to see how others would properly constrain.
        Like • Show 0 Likes0
        Actions
      - Glenn Schroeder @ Bjenk 8100 Jenkins on Oct 28, 2013 8:05 AM
        Mark Correct
        Correct Answer
        Bjenk 8100 Jenkins wrote:
        
        Ok I am getting better at the fully defined stuff to a point. What you think about tools>fully define sketch option. Mine is turned off, but it really doesn't matter because I'm in the habit of only using fully defined sketches.
        
        My strategy right now is figure out where I want my origin to be before I start. Good idea. I don't know what kind of stuff you're modeling, but it there is any symmetry to your parts, it's usually a good idea to keep at least one, and preferably two, planes centered on yur part.
        
        Start my sketch>add dims. Usually its defined. If not, I hit fully define sketch option to see what it adds. That shouldn't be necessary. Unless you've changed something in Options, sketch entities that aren't fully defined will be blue instead of black. However, if that helps you, by all means, go ahead.
        
        THis actually helps me know what the program expects. The only thing it really adds is how far away from origin something is.
        
        Here is a question that would help me out. THere a way to add same feature to more than one entity. For example, if you have five circles all with the same diam. is there a way to define them all at once like the way fully define sketch option does, lol? Ctrl+select them all and apply an equal relation is about the best you can do at present, though I would love to have an option for sketched holes to make them equal when placing.
        Like • Show 0 Likes0
        Actions
        Kelvin Lamport @ Glenn Schroeder on Oct 28, 2013 9:00 AM
        Mark Correct
        Correct Answer
        Here is a question that would help me out. THere a way to add same feature to more than one entity. For example, if you have five circles all with the same diam. is there a way to define them all at once like the way fully define sketch option does, lol? Ctrl+select them all and apply an equal relation is about the best you can do at present, though I would love to have an option for sketched holes to make them equal when placing.
        I agree. It would also be nice for an equal constraint to be applied automatically when copying a sketched circle, polygon or whatever.
        Like • Show 2 Likes2
        Actions
Lenny Bucholz Oct 28, 2013 10:04 AM
Mark Correct
Correct Answer
Bjenk 8100 Jenkins wrote:

Hello,

Drawing a fully defined trapezoid should not be a hard thing or time consuming thing to do. I have been drafting a long time with other programs and never had such problems.

THanks,

Brian
Brian,

First what CAD programs have you used, I ask because we could explain better for the comparision of SW to them.

Making a fully defined Trapazoid is pretty simple if you use the rectangle tool, Once the rectangle is sketched, say the lower left corner is coincident to the origin, add a centerline to the mid points verticaly to the midpoints of the top and bottome horizontal lines, then delete the vertical relations on the left and right lines, pull one of the top end points in towards the centerline and there it is a trapazoid. because of the centerline added to the midpoints you have just gotten symmetry for free and fully defined will happen with some dims after that because you are locked to the origin.

Now I've explained this one way using an existing sketch tool and modifying it to work to save time, what you have to understand is that you may have to just re think how you are to sketch things, if you haven't had a class or a coworker to help you understand you may need to play with other ways to sketch, it just may take you breaking old habits of the others CAD softwares you have learned.

Also include a pic of a sketch shape you are having trouble with so we can help explain how we would start it to help you more.

lenny

Message was edited by: Lenny Bucholz
Like • Show 0 Likes0
Actions

Fully defined

Outcomes

Related Content

Recommended Content