jumping from wrong side of line

AnotherOnshapeUser

Problem happens all the time:

1. Draw a line from the side of line A to the right
2. Specify length
3. line A jumps over to the left !!

how do you stop this?  I would think that if I draw a line starting at point X, and stop it somewhere, and enter a length, it would be SO logical to continue the line or shorten it to that exact length.  I do not want to have to add constraints or a 'fix' to the existing line, I just want Onshape always to add length in the direction I was already going.

This also happens when you are doing an offset: 1. draw an image.  2. Select it and request 'offset' and change the offset distance 3. POOF !  The image jumps over to the side.

Why not just assume that wherever I started was where I WANTED to start?

owen_sparks

Hi.

I'm guessing here as we don't have your example that "Line A" is not constrained, that is to say it's blue on the sketch?  The sketcher will then try to "solve" the requirement of the length of the new line. In this case there are multiple answers to that solve, ie move line a or line b.

If this assumption on my part is true then to stop it happening we want to constrain "line A".  This could be adding a fix constraint or dimensioning to something that is already fixed. If we do that there will be only one valid solution for the solver, so it won't have to guess at our design intent.

Longer term perhaps the solver could have additional intelligence as to the order it tries to solve in, so if we have something unconstrained it'll act more as we imagine.

Does that make sense?  If not, or if I've got my original assumption wrong then please shout.

Cheers,

Owen S.

NeilCooke

@AnotherOnshapeUser can you make a short video showing this?

AnotherOnshapeUser

Owen unfortunately understands the problem all to well.

Instead of click, draw, insert length, click, draw, insert length, which is quite intuitive, one must constrain, click, draw, insert length, constrain, click, draw, insert length, and then remember all those constraints later on when you want to change something.  This is so obviously and so easily a fix it should be done.  It does not require artificial intelligence, just tell the program to remember where you started drawing the line and measure from there it should be a no-brainer.

NeilCooke

@AnotherOnshapeUser I was asking for a video because I am unable to reproduce and I would like to understand the scenario better.

owen_sparks

@NeilCooke
Example

I've made two vertical lines here, each constrained to nothing.

Then added an additional horizontal line to the upper vertical line, which I've entered a length for before committing the line.  Behavior is as desired, the line extended to the right of the screen, leaving the vertical line in place.

Now if we do the same thing to the lower line, but to the left then when we add the length of our new horizontal line it still grows to the right, pushing our vertical line to the right.

The solver is doing it's job, but I agree the intuitive thing here would be to extend that line to the left of the screen and not move the vertical geometry.

Link to file

Cheers, Owen.

AnotherOnshapeUser

Owen:

thanks for the detail.  Tell me!  Does it ALWAYS move to the right?
thx

NeilCooke

OK I can see that now, I was just doing the draw to the right bit as per the OP. Seems it is always keeping the leftmost point static then applying the dimension. Not sure if this is something we have control over (we could possibly add a temporary constraint, solve, then remove but would that work for every scenario and not upset other users? Probably not). @AnotherOnshapeUser you can "contact support" under the help menu to raise a ticket against this, but if this is driven by D-Cubed (the sketch solver) then we may not be able to change this behaviour.

AnotherOnshapeUser

I've run some tests and I cannot tell whether it will move the beginning or the end of a line according to any order.  Seems like horizontal line moves in Y, and a vertical line in -Z, but that could be because of something else I did.  At least it would be nice to know when to worry about messing up work you already did....

AnotherOnshapeUser

Wow Neil you really know the insides of Onshape.  Is D-Cubed outsourced or otherwise not reachable?

NeilCooke

If you look at Help/About you will see that D-Cubed as well as Parasolid are owned by Siemens PLM. These are pretty much industry standard (SolidWorks uses both these as well as Solid Edge and NX) and we license their technology.

AnotherOnshapeUser

Yes D-Cubed is made by Siemens and must somehow be integrated into Onshape.  Not such a no-brainer after all...oh well. 

The big problem with this is that a drafter can work for an hour on a sketch, and then add a line and not notice that the starting point jumped and changed the sketch, and then incorporate errors into the job.  Have to watch it like a hawk!  

owen_sparks

Just another thing to add.

I'm by nature a "ranter".  I take physical pleasure in shouting about things that annoy me.  Maybe it's because I'm British, and we like complaining...  I'm also not shy in telling Onshape about things I don't like.  (In a polite constructive way of course, see note on being a Brit.)

All that said the behavior above does not annoy me in the slightest, because either:-

(a) Un-constrained geometry is just plain bad, so I'll have already constrained the entity I want to add to, so the solver will do what I want.

(b) If I've not constrained the geometry I'm adding to it's because it doesn't matter where it is, so if it moves to the right or left is of no consequence.  Chances are I'll still constrain it at the end anyway, because blue geometry = bad geometry.

At the start of using Onshape a mental hurdle was constraints. Once grasped they're pretty intuitive to either add explicitly or on the fly by "waking up" points that you want to constrain to.  Now like them a lot.  It's a little logic puzzle to fully constrain a sketch, and more importantly constrain it in a way that allows it to be edited in the future and react as intended.  Ie "design intent".

Right, I'm off to find our which dev thought it would be great if every C# line of code needs to end with a semicolon...

Cheers, Owen S.

 

AnotherOnshapeUser

Thanks for the kind words, Owen.  I'd be glad to learn how to use constraints better.  Can you please explain how to 'wake up' points you want to constrain?

I've had a lot of trouble with constraints.  Often I think I've got a sketch tied down and then Pow it jumps all over the place.  Do I really have to constrain every end of every line?  How can I do it easily?

Jake_Rosenfeld

@AnotherOnshapeUser

This may help: https://learn.onshape.com/courses/fundamentals-sketching

john_mcclary

owen_sparks said:

All that said the behavior above does not annoy me in the slightest, because either:-

(a) Un-constrained geometry is just plain bad, so I'll have already constrained the entity I want to add to, so the solver will do what I want.

(b) If I've not constrained the geometry I'm adding to it's because it doesn't matter where it is, so if it moves to the right or left is of no consequence.  Chances are I'll still constrain it at the end anyway, because blue geometry = bad geometry.

Cheers, Owen S.

 

Agreed, In my opinion: this is something all new users of ANY parametric cad system MUST learn before all else!
Please take your time @AnotherOnshapeUser and master 2D sketches and constraints. They are the foundation of your entire model.
One blue line can set you back hours of chasing your tail trying to fix a very simple problem down the road.

Whether or not you must constrain the line at the beginning of your work flow, or at the end, makes no difference. Before you close a sketch you should ensure all points and lines are Black anyway.

Constraining early will also make your life easier in many ways, for example: any time you construct geometry with circles and tangents. They will turn your sketch inside-out with even the slightest over-drag of the mouse. Sometimes the only recovery is to delete the circle/arc and re-sketch it. That's just how it works. How can the software truly know what direction you intend a line to extend? Should it record every mouse click and pixel location you mouse was like a movie, so when you come back to it a week from now it will know you intend to extend left instead of right? Sounds far fetched when you think of it that way right? But how else could it work? will it need to remember the creation time of each entity so the earlier entities drawn are "less movable" when adding dimensions to new lines?

There is a old saying that I haven't seen proven wrong yet in computing: Garbage in - Garbage out;
Computers are dumb, WE are what make them do the amazing things.

billy2

constrained vs. unconstrained, this is a good thread.

An entry level designer needs to understand this and it's not easy. More time needs to be spent here on the basic sketch concepts. It's not easy for new users. You can't short cut this conversation without having further problems later on.

In a sketch, black is good and blue is .......? Depends if you know what you're doing.

Turn constraints on and try to understand how the constraints work. Onshape has a lot of automatic stuff like picking up horizontal & vertical to origin. Some times I think it's too sticky.

It's not drafting, there's a lot more to it. Design intent, what should the sketch do?

D-cubed is nothing more than a linkage solver. Draw a four bar linkage and spin the driving link. It works perfectly the way it should.

john_mcclary

billy2 said:

Onshape has a lot of automatic stuff like picking up horizontal & vertical to origin. Some times I think it's too sticky.

I used to think that too, until I learned holding shift while sketching or dragging will turn off the auto-constraints
Been using parametric CAD for over 10 years, still something new to learn even on the basic sketching tools.