Parallel constraint issue

[Anonymous]

Hi,

I cannot make the small line (inside the red circle in the attached picture) parallel to the longer black line next to it (indicated with the arrow). Please let me know where I am going wrong with this sketch because I cannot use the equal constraint on the circles either.

Kind regards

Michael Mullineux

[TheCADWhisperer]

Simplify your sketches and your life will be easier.

This should be several sketches.

Also, is there a logical reason that you are not working with symmetry about the origin?

[Anonymous]

Hi CW,

I am not sure what you mean by simplify the sketch by splitting it up. How would it help if I split it up, I still need to reference other lines (parallel and equal constraints). Please could you explain a bit more.

The pattern is not symmetrical (I am planning on mirroring it as that part is symmetrical about the vertical middle line). how would you use symmetry to simplify this sketch?

Do you know why I cannot make that small line parallel to the longer line?

Kind regards

Michael Mullineux

[TrippyLighting · Accepted solution]

I've used a similar approach to your sketch in previous projects but it has one Achilles heel. The Fix constraint often interferes with other sketch operations and in this case, that is the reason that you cannot make these 2 lines parallel.

If you remove all Fix constraints you'll find that the parallel constraint will work.

If you don't use the Fix constraint, however, you'll likely run into another limitation of the sketch engine. As you add spline points and more splines the are all not constrained and dimensioned Fusion 360 will get more and more sluggish in UI responsiveness. 

The way around this is to consider a sketch really only as a basic building block for 3D geometry so:

1. Break this sketch into objects that represent a closed profile> that might be 10+ sketches for this object.

2. Uses fewer spline points and work with the length, and orientation of the tangent handles.

3. Do NOT mirror an entire sketch. Create half of the 3D geometry and mirror 3D geometry. Same for patterning. A hand full of mirrored or patterned instances is OK but not an entire sketch.

All the above will result in much better performance.

[Anonymous]

Hi TL,

Long time, thanks for responding.

I figured the fixed constraint was causing the trouble but what I dont understand when about it (ie this part of your reply "The Fix constraint often interferes with other sketch operations and in this case, that is the reason that you cannot make these 2 lines parallel. If you remove all Fix constraints you'll find that the parallel constraint will work.") is that I have applied the fixed constraint to only one of the lines, so in my head it should be fine to use the parallel constraint because it will make the unconstrained line parallel to the fixed constrained line. I think I am missing some basic understanding because at the moment I cant see logic to what is happening and it must have a logical reason. I really struggle to accept, use or grasp something if i dont understand why it is happening.

I will use the tangent handles in future to minimize the number of spline points in my sketch but how do I fix spline lines without using the fix constraint? I saw this method on a youtube video and that is why I am using it, but I wouldnt know how to constrain such complex and curved shapes with the regular dimension/parallel/tangent/etc constraints. I will follow your 3 pointers in future but how do I go about drawing and constraining these shapes the correct way?

If there are any videos or forums that you know of that already show this please just drop me the link so you dont have to answer a question that has already been answered.

Kind regards

Michael Mullineux

Kind regards

Michael Mullineux

[TheCADWhisperer]

If it was my design - I would start over using robust techniques.

Step 1. Attach your canvas image file here.

[Anonymous]

Hi CW,

Id appreciate all the help with learning a more robust technique you could give me. attached is the canvas pic.

Kind regards

Michael Mullineux

[MichaelT_123]

Hi Mr TippyLighting,

Excellent analysis and pieces of advice...

May I add some point here?. Of course, I may!

Splines are very vibrant, challenging to handle because they have so many degrees of freedom. (remember when you has (had) been a teenager?)

Constraining them rigidly as in the current F360 sketch engine can create a deceptive, stubborn case we evidenced here, requiring the serious intervention of authorities.

F360, it is the TYRANNY.

F360 algorithm policymakers, give splines what they want!

 “FREEDOM FOR SPLINES - WE WILL NOT TANGENT EASILY”

If I could be adviser here, build-in additional option for splines fixing/unfixing the first derivative (possibly separately higher ones).

This would allow to switch on/off tangentability at their ends. Additionally, such change would also enable a path to facilitate the option to tangency (within range) ‘inside’ splines by relaxing the first (and/or higher)  derivatives without changing fitPoints positions.

Just imagine a spline sticking willingly to a lovely entity in its proximity,  ooohhh.

As the result, you would have “a vibrant spline”, behaving within reason and you (F360) without being forced to resort to TOTAL CONSTRAINOCRACY.

Regards

MichaelT

P.S.

… for Michael Mullineux.

This seemingly trivial case has pointed to quite important constrain's algorithmic issues.

From now on, you can call yourself ‘Michael Who Moved Constrain' 

Regarding “Michael”,… “Michel” and “Michał” are also awesome.

[TheCADWhisperer · Accepted solution]

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@Anonymous wrote:

Id appreciate all the help with learning a more robust technique you could give me. attached is the canvas pic.

 There is nothing wrong with having 20 simple sketches in a part.

[TheCADWhisperer]

@Anonymous 

Where did you go?

[Anonymous]

Hi Michael,

Thanks for the feedback, I really appreciate all the feedback and help from everyone. I may have missed it but I am still none the wiser as to why i cannot make the short line parallel to the long one, can you tell me why that is happening?

Kind regards

Michael Mullineux

[TrippyLighting]

I thought I'd already explained that 😕

The Fix constraint on some of the sketch objects seems to interfere and prevents you from creating the constraint. That is a bug in the sketch engine.

Did you read my reply ?

I provided a few steps how to circumvent the bug e.g. break the sketch into several smaller sketches.

[Anonymous]

Hi CW,

Thanks for the video, I will make sketches with fewer closed loops. I have a few questions though;

1. how did you know that you projected more than just the line of symmetry? 
2. if you project a line from a different component and then move that component to make a joint, how does the projected line get affected?
3. The 3 rectangles you drew dont quite get the shape of that golden line (the 2 end bits are at angles) so there I think I would use normal lines and then either the fillet tool or curved lines for the edges
4. Can you please show me the more robust method of drawing the curvy shapes as well?

Thanks again for your effort (unfortunately my day job interfered with this last night so I could only reply now, sorry about the delay)

Kind regards

Michael Mullineux

[Anonymous]

Hi TL,

I did read your reply but had a question on it

"I figured the fixed constraint was causing the trouble but what I dont understand when about it (ie this part of your reply "The Fix constraint often interferes with other sketch operations and in this case, that is the reason that you cannot make these 2 lines parallel. If you remove all Fix constraints you'll find that the parallel constraint will work.") is that I have applied the fixed constraint to only one of the lines, so in my head it should be fine to use the parallel constraint because it will make the unconstrained line parallel to the fixed constrained line. I think I am missing some basic understanding because at the moment I cant see logic to what is happening and it must have a logical reason. I really struggle to accept, use or grasp something if i dont understand why it is happening."

If only one line is 'fixed' why doesnt the parallel constraint make the unfixed line parallel (ie why doesnt the small blue line move) if this is a bug in fusion then Ill just wait for the next version and see if the problem is fixed but if it is a mistake in my understanding then I would like to remedy it.

Kind regards

Michael Mullineux

[TrippyLighting · Accepted solution]

There is really no misunderstanding or fault on your side. This is a long standing bug in the Fusion 360 sketch engine and the only thing you can do is to avoid using the Fix constraint.

Sometimes it works OK, but sometimes it interferes. I don't have a better explanation for it either.

[TheCADWhisperer · Accepted solution]

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@Anonymous wrote:

3. The 3 rectangles you drew dont quite get the shape of that golden line (the 2 end bits are at angles) so there I think I would use normal lines and then either the fillet tool or curved lines for the edges

4. Can you please show me the more robust method of drawing the curvy shapes as well?

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 3. I was simply demonstrating that you create many simple sketches rather than one massive monolithic sketch.  My intention was not to take the time to reproduce the "art" of the design - that is up to you.

4. See #3  As @TrippyLighting noted - use as few nodes in spline as possible and manipulate the Handles.  I think it is OK to use Fixed constraints on these nodes as long as the splines are in sketch by themselves.  Bottom line - several simple sketches rather than one complex sketch.  The line/arc geometry you can get away with several profiles within one sketch, but especially for the spline profiles I would do a sketch for each one.

[Anonymous]

Hi TL,

Thanks for the explanation. 

Kind regards

Michael Mullineux

[Anonymous]

Thanks CW for the help.

Kind regards

Michael Mullineux