Getting to "fully defined"

thomas_holford

Reference document: Octagonal pedestal - multipart

https://cad.onshape.com/documents/28044d76fae64781bc7c9c46/w/f0b392a79f784531824bf25d/e/f31eb6eef1ea46ceb4d1ee03

Part Studio: Parts Rev 2
Sketch 1

I've created an octagon shape with two lines using offset.  To this point, the sketch is fully defined.

I added a box at the 9 o'clock position using the corner box tool.  The box is related to the inner line of the octagon.  The sketch is still fully defined.

I copy the box 8 times (7 replicas) using the circular patter tool.  The original box remains fully defined, the 7 replicas are NOT fully defined.

I try adding additional relationships to the box at the 10:30 position and succeed in fully defining the box sides but not the whole box.  Trying other relationships over defines the entire sketch.

Help.  What is necessary to define the replicas without over defiining the whole sketch.  OnShape seems to report what relationships exist, but is not very helping in saying what additional definitions or relationships it wants.

3dcad

@thomas_holford
The problem was that the middle point of circular pattern was not constrained to origin.

The easy way to test constraints is simple trying to drag things around and see what is moving. See the image below.


Here is fixed version. All I did was coincident constraint between origin and middle point of circular pattern and deleted one over constraining dimension.
https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/07fb12e6529d41ed9783a904

jakeramsley

When making a circular pattern, the system originally guesses the center of rotation as the origin but doesn't apply a coincident constraint if it isn't moved.  This is to reduce the need to delete a constraint if the guessed position isn't correct.  Next time, if you want it to be coincident with the origin, while creating the circular pattern move the center around a bit until there is a coincident snap to the origin.  At this point, the center of rotation will be constrained to the origin.

3dcad

@thomas_holford
The problem was that the middle point of circular pattern was not constrained to origin.

The easy way to test constraints is simple trying to drag things around and see what is moving. See the image below.


Here is fixed version. All I did was coincident constraint between origin and middle point of circular pattern and deleted one over constraining dimension.
https://cad.onshape.com/documents/d29ff8e74a0f49809e533f48/w/48fedb2064cc4f30a27ee6e8/e/07fb12e6529d41ed9783a904

jakeramsley

When making a circular pattern, the system originally guesses the center of rotation as the origin but doesn't apply a coincident constraint if it isn't moved.  This is to reduce the need to delete a constraint if the guessed position isn't correct.  Next time, if you want it to be coincident with the origin, while creating the circular pattern move the center around a bit until there is a coincident snap to the origin.  At this point, the center of rotation will be constrained to the origin.

thomas_holford

Thank you.

What I am taking away is that for anything to be fully defined, it has to have a constraining relationship to the origin.

Correct?

jakeramsley

thomas_holford said:

Thank you.

What I am taking away is that for anything to be fully defined, it has to have a constraining relationship to the origin.

Correct?

Not technically.  It needs to have a definite position in the sketch which requires either a fixed constraint (forcing it to be where you put it) or to have some kind of relationship to something that is outside of the sketch.  For example, you could have made the exact same sketch that was about the vertex of a face and as the face has a well defined position then the sketch would be fully constrained.

1. I made an arbitrary located rectangle in sketch 1.  The lines and vertices are blue because they are under-defined.  This means that their position isn't fully defined and I can grab and move them.  I will save this sketch being under-defined.


2. On a new sketch, I dimensioned a rectangle relative to the rectangle on sketch 1.  As far as sketch 2 is concerned, sketch 1 has been committed and solved, the position of the first rectangle is fully defined.  Because of this, I have defined my new rectangle off of the sketch 1 rectangle and it is fully defined.  There is no relationship to the origin here.


3. If I go back to sketch 1 and move my rectangle, the sketch 2 rectangle will move accordingly.  It is being solved after sketch 1 is solved relative to the rectangle in sketch 1.

andrew_troup

Great example, @jakeramsley , thanks
It goes well past answering the immediate question, to clarify something much more fundamental.

Your third step is also a great example of non-trivial, non-obvious pitfalls from leaving sketch geometry under-defined.