Fully Constraned to Itself

[docara]

Hello all,

Is there an easy way to Sketch a shape (which is has a double symmetry) which is constrained or locked to itself, but overall needs to be moveable and/or rotatable so it can be positioned - initially by eye, before the final position and an extrude performed.

I seem to have done it with LOTS of dimension lines across diagonals etc but PC's not happy, if you move the sketch occasionally if 'forgets' the dimensions. there must be a better way

thanks

Matt

[laughingcreek]

In general, yes.  You can do that.  You want to be smart about what you dimension, and not do it willy nilly.  I'm not sure, but I suspect using constraints over dimensions where possible will give better performance.

Post an example, you might get some help. 

[laughingcreek]

well, never mind.  that process seems to be rather buggy.  a work around would be to put the sketch in a component by itself and move the component around.  that does work pretty good.

@jeff.strater, could you take a look at this screen cast.  It shows what looks like 2 different bugs in sketch engine.

[TrippyLighting]

I am not are those are bugs or conscious decisions by the developers for Fusion 360 to respond that way.

For example, make a 2 corner box NOT starting at the sketch origin.

If you rotate that using the move tool then it deletes the horizontal/vertical constraints.

There are valid arguments to delete them, or not to delete them.

[laughingcreek]

Ok, I see what your saying. However, I would argue that in your example the sketch should not have rotated, instead of breaking the constraints.  If you use the linear move transforms on a constrained sketch, nothing will move. (I wish there were some visual feedback on why it won't move, but that's a different discussion.)  It only breaks constrains or dimensions when the rotate move transform is used.  That's inconsistent at best.  Personally, if I manually place a constraint, I would like it to stay there unless I remove it. 

[docara]

Just some feedback.

Yes - I was guilty of dimensioning 'willy nilly' and using constraints.

It was in a component!

What I was trying to do a panel cut-out with for satellite mounting holes, and I wanted the sketch to be the basis of a Cut Extrusion when the position was finalised. We are perhaps SO used to Sketch >Extrude type workflow that I wasn't seeing the 'wood for the trees',  I 'solved' the issue by a little lateral thinking.

I constrained the shape the best I could but making sure not to use Vert/Horiz constraints because the eventual cut-out was going to be on an angle. I locked it down - not to the nth degree but good enough. I then extruded it so it was a body. This now made something much more able to useable and less likely for the Sketch lines and arcs to move around. I then used this body to position it where need and I then just extruded again to cut my hole.

Matt

[laughingcreek · Accepted solution]

great, glad you worked it out.

with the component idea, you move the component itself, not the individual sketch in the component.  Is that what you were doing?  That work flow shouldn't effect the sketch in any way whatsoever.

[docara]

Ah! I see what you're getting at.

No I realise I was trying to move the sketch by clicking on it at and trying to drag it around NOT moving the component itself

[chrisplyler]

I have sketched/constructed holes/cutouts that are self-contained and only dimensioned/constrained around their own "origin" that I made out of crossing, perpendicular construction lines.

So the "crosshair" of construction lines, and the sketch of the hole along with it, can be dragged freely around the sketch. Only later, when the final position of the hole is known, you just put in the final dimensions from the crosshair to other edges or the component origin or whatever.

Here is an example I did a few weeks ago, so you can see what I mean...

[docara]

Hi Chris

Yes that was the sort of thing I was trying to do but my cut-out was not an off-square square, I had four 'wings' + various radii, so I realised, after posting my original question, that it was never going to work smoothly.

Thank you for your trouble sorting out a Screencast, much appreciated.

Matt

[chrisplyler]

As long as you can fully constrain everything to that crosshair properly, the shape doesn't matter.

I deleted the hor/vert constraint I had, and added a parallel constraint to do the job instead, and now I can move the thing around and rotate it freely too. The main hole and the screw holes all move as a unit and don't get messed up no matter the movement. They act as a self-contained unit within the sketch. When I'm ready to lock it down I just dimension the center point in X and in Y, and give one of the lines an angle, and I can lock it wherever I want it to be.

[laughingcreek]

Part of this exorise was being able to rotate the sketch with the move command.  What happens to your sketch when you do that?

[chrisplyler]

Um... what do you THINK happens when I rotate it with the Move tool?

[laughingcreek]

Interesting.  I wonder why it sometimes deletes the dim?

[chrisplyler]

I don't know why. Yeah, when I did it like you and then rotate some dimensions are lost.

I also don't know why you are able to dimension two of the corners, one of the sides, the distance between the two sides, and then dimensioning the other side doesn't over-constrain the thing. Geometrically, my mind is telling me it should be over-constrained. In fact, when I do it, that last dimension becomes a DRIVEN dimension.

Anyway, if you do what I said about locking it all to a crosshair of construction lines, then it works without losing dimensions.

[laughingcreek]

seems to be particular about what and how you select when placing dims.   Hoping someone from AD will weigh in.  @jeff.strater?

[jeff_strater]

Basically, the answer is that Fusion tries to preserve as many dimensions as it can.  If a dimension is an "aligned" dimension, it can be preserved.  If it is a horizontal or vertical dimension, it has an implied horizontal constraint to that dimension, so it cannot be maintained:

The dimension on top is aligned, while the one on the bottom is horizontal:

If I select and rotate the whole thing, only the top one can be maintained:

Constraints behave similarly.  Perpendicular or parallel constraints can be preserved on rotate (assuming both lines are selected), but horizontal or vertical constraints will be removed.

[chrisplyler]

Okay, that matches with the behavior I've seen. If I rotate that figure slightly, and THEN dimension it in such a way that none of them are vertical or horizontal, THEN they won't disappear on rotation, even if they are rotated such that those dimensions BECOME vertical/horizontal and then rotated away again.

That's kind of a dumb way to set up dimensions. Or at least it's a limiting way.

The hidden constraints of dimensions ought to be things like "parallel to that line I'm showing the length of" or "perpendicular to those two parallel lines I'm showing the distance between" or "parallel to an imaginary line between those two points I'm showing the distance between." Well, those and the things like witness line length, text position along line, etc., as required to maintain the relative position established by the user. In this way they could be maintained despite rotating the whole figure.

They ought not have any constraints other than to the items they are relative to. Constraints to vertical/horizontal serves no useful purpose and is in fact limiting.