Stumped: Cannot Fully Define Sketch
Hello, @Anonymous.
I tried to fully constrain your sketch, and I noted two things:
- I applied a vertical constraint to your symmetry line, which constrained the top part of the sketch;
- I added a dimension of 1/8" between the narrow areas of the sketch, which constrained the other entities.
Let me know if these two actions keep your design intent.
Here is simplified version with no construction geometry. Using equal helps simplify also.
I think your trouble stems from duplicate entities.
Overlapping lines are covering unconstrained untied duplicates.
If you are making duplicate dimensions, then an equals constraint can replace it, making it clean and easier to read.
I deleted all the construction lines, (6 or 7 of them)
The top line of the sketch is a pair of half lines??.
Might help.
In the file that you attached there are unconstrained construction lines that you don't really need anyway so you can actually delete all the construction lines as they aren't really needed. You also don't need all of those dimensions, use equal, coincident and tangent in place of some of the dimensions.
Here is the way I would draw it.
Accepted solution
HI Marty,
I think everybody in in this thread has give some good advice and I hope you are able to get to the result you want.
I'd like to share a bit of my perspective on this (much of it is already represented by others here), but there's a few things to consider when using any 3D parametric CAD modeler.
- Keep you sketches as simple as possible, remember Mies van der Rohe said "less is more." This is the philosophy to take when it comes to your sketches.
- What's the least amount of information you can provide to create the 3D geometry
- Don't try to cram everything into one sketch, when you run into problems (and you will at some point) it's much easier to trouble shoot the root of the problem when your sketches are simpler
- Remember the production drawings, like the one for the link bracket are for a fabricators/manufacturers to make the part from. When building CAD models, the sketch isn't always going to replicate the drawing you have in hand (or on screen)
- Much of this comes from experience, and there's almost always more than one way to get there.
- Look at the problem and how do you distill it into its simplest geometric shapes and forms.
With that said, If I were to look at your sketch as an instructor, the things I see are typical new to cad workflow problems. You did a good job getting the shape right and dimensioned. The one thing I'd say about your sketch is it's over complicated, too many duplicate dimensions, too many unnecessary construction lines, disconnected geometry (the white dots) and it's hard to determine if that's some of the extra construction geometry or the curves you actually want to make the 3D part from.
When I look at the break down of the drawing I see it like this:
the magenta curves are your critical dimensions and the green are resultant geometry
Following to a sketch that looks like this: there's a number of constraints not shown in this image (I'll attach my version so you can understand what I did here). This is very, very simple. I intentionally left the holes out, because I'm using the hole command in the modeling tools to do that, I just need center point locations
Again, the response from other folks in this thread I know were helpful, I just wanted to give a bit more insights into the why/how to approach a sketch like this.
hope this helps,
Jamie Gilchrist
Senior Principal Experience Designer
Jamie Gilchrist
Senior Principal Experience Designer
First you have white points, and some on the outline, they should not be there.
Next you would be served well to dimension or make things coincident to the origin, lining up is not good enough.
Sketch articles should be constrained and then dimensions for size.
Unless you have to use mirrors in a sketch, this is all you need, and mirror twice in the modelling window.
Might help...