Sketch Arc is Preventing Squares from Resizing Properly

[oo7_golden_1]

Hello 360 community! I accidently posted this issue in the wrong forum section the other day and another community member was nice enough to direct me here.

I am trying to create an adjustable model based off of a Fibonacci spiral. I drew up a quick sketch of a Fibonacci spiral, tested it to make sure that it was constrained and adjustable and everything seemed to work as expected. When I started building it again I cannot seem to get all of my arcs to work correctly.

The model is fully constrained as it should be, but when I adjust my initial square’s size (which I built the sketch off of) Fusion errors and tells me to check pretty much everything in the model.

After some deleting to try and pinpoint the issue, I believe I have narrowed it down to some Arcs causing the problem.

It’s strange because some arcs work and some do not. I have uploaded the model to demonstrate.

To replicate the issue, adjust d1 (found on the smallest square next to the origin point) notice how the model adjusts, then add an arc (I used 3 point arcs) into one of the empty squares to try and add to the spiral. Then after drawing the arc try adjusting d1 again. Instead of adjusting as it should (like the other squares with arcs) it seems to break the render and cause fusion 360 to fail at the computation.

As you can see the arcs SHOULD also adjust accordingly. The empty squares should allow similar arcs but if I add arcs to those squares the arcs ARE constrained but they prevent d1 from being adjusted.

I tried using a fit point spline instead of arcs but the spline does not stay within the squares, and sometimes doesn’t seem to render properly and I need the model to be precise.

Does anyone have any creative advice on how I can build this properly? Or on why I cannot seem to add arcs to the squares in question without the arc causing resizing problems later on down the road?

[brink.gregory · Accepted solution]

Hi,

I had similar issues when I created a sketch that had a bunch of cascaded dimensions.  When I would change a user defined parameter the calculations would bomb because everything was referenced to something that had to be pre-calculated.  I recreated the sketch so that all of the dimensions are from the origin and it worked fine.

The other issue here is that the sketch is effectively overconstrained.  I deleted all of the dimensions and then added the minimum number necessary to get the drawing fully constrained.    This was an interesting process because some of the construction lines get the constraint from the tangent and some from the reference frame dimensions.

I've attached that version so you can see how it works by just changing the single user parameter.

Good luck!

[etfrench · Accepted solution]

Try it like this:

[laughingcreek]

I mean, it could be that your just overloading the sketch solver.  a few things to implement-

-you don't need the diagonals, just more stuff for the solver to deal with.

-use individual lines instead of the square tool, and then avoid laying multiple lines on top of each other.

-you only really need the one dimension, do the rest with constraints.

or

do away with the squares all together-

[TrippyLighting · Accepted solution]

When sketching in Fusion 360 I try to avoid construction lines if I can replace them with constraints, the horizontal vertical constraint in this case. This sketch does not contain a single construction line :

[TheCADWhisperer]

@oo7_golden_1 

I posted The Solution in your original discussion thread.

Did you examine the file?

I always insisted that my students use construction lines - going all the way back to the drawing board in the last century.  Helps to visualize Design Intent.

[oo7_golden_1]

OK, I owe a second apology to @TheCADWhisperer, who took the time to also create a fusion 360 sketch for me and due to a misunderstanding on my part I saw his images but missed the fusion file that he uploaded for my benefit. So, sorry for that CADWhisperer. 
I am going to upload his design here, mark the other thread as solved and continue the discussion on this thread where I should have posted it originally. 

OK, where to begin...
I am still a Fusion 360 layman and I have some questions...
Lets start with the file that TheCADWhisperer supplied first which I am going to upload here (incase another user needs to reference it in the future). 
TheCADWhisperer... how you built that sketch is making me feel more and more like a novice by the second. So lets break it down so that I can wrap my brain around your process. 
I assume that you drew the smallest center rectangle first and then converted its lines into normal construction lines and then built everything off of it as I did...
How did you apply the "Start_Radius" to that square? For my first square I selected the top side of the square and pressed D to give it a sketch dimension of d1 at 2mm. Then I selected the side of that square added a sketch dimension (d2) and clicked the d1 dimension so that d2=d1 and both sides of the square remain the same (an equal constraint can do this as well). I learned to do this through trial and error when first getting into fusion 360... so there is probably a cleaner solution being demonstrated by you here but I will need you to educate me as to how you did it as I am not sure what you did.
I also see that there are polygon constraints in the center of each square... are you creating circumscribed polygons instead of center rectangles?
I am not even sure if you selected both sides of the rectangle/polygon and then press d to create a sketch dimension because its not labeled with a "d". Is it a dimension and you simply renamed it to "Start_Radius"?
What kind of Arc type did you use to create your spiral? 
I think your rectangles/polygons are sized incorrectly as well because each larger square should have one of its sides be equal to the sum of two sides of the last two smaller squares... if that makes sense. The two smaller squares should, when placed adjacent to one another, have a combined length equal to the next largest square...
I tried to do this in my sketch by making the next largest squares size equal to the sum of one side from each of the two previously created rectangles. I hope I am explaining that well enough.
I am also not even sure how your rectangles are being resized as I see no sketch dimensions attached to them...
I am a very visual person and I cannot seem to see how you built your sketch. Will you please cure me of my ignorance? If I can learn some good sketching practices for future projects I would be most grateful.

[oo7_golden_1]

@TrippyLighting
What kind of sorcery is that! 
That is pretty creative... so you drew a 3 point arc... constrained one of the end points to the origin, then put a horizontal constraint between the point of the arc not attached to the arc line and the point of the arc line not currently attached to anything in order to constrain it 90 degrees... then used the arc radius as your sketch dimension and when creating a new arc you add the length of the previous two arc radius sketch dimensions.  
Hum...
Because of its constraints you can even select the entire sketch, copy it, complete the current sketch, create a new sketch, paste it into the new sketch and constrain the first ark to the origin point of the new sketch and everything automatically locks into place and the sketch becomes fully constrained.
Very, Very CLEAN. Hum...
Now that I think about it... what types of arcs did you use in your sketch? It appears to work for both 3-Point and Center Point Arcs. Do you remember what type you used? Do you prefer one type over another?
So far this might be my favorite solution as I should be able to go back into my original sketch, delete all the lines, constrain everything, and be good to go... 

[TheCADWhisperer]

@oo7_golden_1 

You can set the sketching to be Construction before starting - no need to convert.

Dimension. Select one side of the Polygon and type Starting_Radius=2 as an equation variable=value. 

I started out with Centerpoint arc but Fusion didn’t automatically add Coincident to the Centerpoint so for the rest I used 3 Point being careful not to automatically add a Tangent (a computationally expensive and potentially confounding constraint as Tangent could have multiple solutions).  I then added Coincident constraint to Centerpoint of arc.

For each succeeding Polygon (polygon assumes equal sides so no Equal (=) constraints needed and no Horizontal, Vertical or Parallel needed either.  Sketched in space at any size and angle.  Added Coincident constraint at one corner to existing previous Polygon and Shift select Midpoint (this is the key) to other end of previous Polygon. The Midpoint assures that each successive Polygon is twice the size of previous Polygon without adding any dimensions. Geometry is geometry.

[oo7_golden_1]

I think you might be right about overloading the sketch solver @laughingcreek. My sketch is pretty complex with a lot of things built on top of one another. 
Your uploaded file is a lot like the one @TrippyLighting suggested.
Will you teach me what method you are using to cause the arcs to adjust themselves? Are they simply adjusting because of the tangent constraints applied to them? 
I tried reverse engineering your uploaded sketch file and I could not really figure out how you added new arcs to the sketch or what is causing them to adjust properly as there are not really any dimensions other than your d1. 

[oo7_golden_1]

Ok, so you created an inscribed polygon with 4 sides and as the polygons radius input instead of just typing in 2mm and then pressing enter and having fusion assign it the name "d1". You typed "Start_Radius=2mm"?
So, "Starting_Radius" became the name of the dimension instead of d1 and the "=" gave the dimension an expression/value of 2. That makes sense.

You do not recommend using tangents for this particular application because the end computation could be quite taxing and cause computational issues. Maybe this is one of the problems with my original sketch as I made sure each arc had a tangent constraint attached to it.

Ok, you said you “added Coincident constraint to Centerpoint of arc”… so you drew the arc, with its starting/first point attached to the end point of the previous arc (and corner of the polygon) and then you placed the second point of the arc onto the other side of that same polygon which automatically created the coincident constraint… then you used a coincident to constrain the center point of the arc to the third corner of the polygon which fully constrained the arc.

“For each succeeding Polygon (polygon assumes equal sides so no Equal (=) constraints needed and no Horizontal, Vertical or Parallel needed either.” Using a polygon negated the need for additional constraints… very clever.

Then you selected the side of the polygon that was to be adjacent to the previous polygon, selected the midpoint constraint and clicked the corner of the previous polygon so that the corner was in the center of the newer polygon. Ok, I am with you.

By using the midpoint though the new polygon is double the size of the previous polygon, as you intended, BUT to be a true Fibonacci Spiral the newer polygon is not supposed to be twice as large as the previous polygon, it needs to be the length of the previous polygon plus the distance/length of the polygon created before the previously created polygon. Side of polygon 1 + side of polygon 2 = side of polygon 3. Does that make sense?

I guess my next question is… How do you set fusion to create construction lines by default?

[oo7_golden_1]

Ok that is pretty close to what I was originally doing except you built your arcs separately and attached them to the model, you used center point arcs instead of 3-point arcs, and you avoided any tangent constraints. I have a feeling that the tangent constraints in my sketch are causing some of the problems. Thank you @etfrench. 

[TheCADWhisperer · Accepted solution]

---

@oo7_golden_1 wrote:

I guess my next question is… How do you set fusion to create construction lines by default?

---

[TheCADWhisperer]

@oo7_golden_1 

I figured out an easier technique - I will make video in a couple of hours.  Check back later.

[oo7_golden_1]

Hi Brink,

I see what you did, cleaning up all of those dimensions and some of the constraints must have been a real chore, thank you for the time you spent to try and help me. I appreciate it.

That being said, I was not sure if your formula/method would work originally because the second square in your model’s sketch was off. An equal constraint seemed to fix that though… and it looks like it should work… Ill have to play with your sketch a little bit more.

Thank you @brink.gregory.

[oo7_golden_1]

Well that is pretty strait forward. Add, sketching with construction lines to the list of things I learned about fusion 360 today. 
Thank you @TheCADWhisperer 

[oo7_golden_1]

"I figured out an easier technique - I will make video in a couple of hours.  Check back later."
I look forward to seeing what you come up with @TheCADWhisperer.

[TheCADWhisperer]

@oo7_golden_1 

The efficient sketching of a Fabonacci spiral is an interesting topic, but before I take the time to create a video on what I think is the most efficient technique -

1.  what is your Design Intent for this?

2. Are you aware that there is a Spiral tool already built into Fusion 360?

[oo7_golden_1]

Hey guys,
@TheCADWhisperer I do not think a coil would work unfortunately. I would like it to be flat for a more 2d-ish artistic project I am planning to 3d print.

I loved seeing all of the ways some of the wonderful people in the community showed how they would build a Fibonacci spiral. Seeing multiple creative ways to solve a problem from many different points of view gives me lots of joy for some odd reason.
So thank you @brink.gregory @etfrench @laughingcreek @TrippyLighting @TheCADWhisperer for all of your wonderful suggestions.  

I chose to model my spiral off of @TrippyLighting. I really liked the simplistic design and I was able to go back into my project and easily apply it, which was a bonus.

Does anyone have any advice on how I can divide the spiral into sections, while still maintaining the ability to adjust the size of the spiral?

I am going to 3D print the spiral in multiple pieces and so I created an offset of the spiral, drew lines, added coincident constraints to lock the lines onto those offsets, and then constrained each line to the origin, and then drew a construction line down from the origin to use as a reference when applying degree/angle sketch dimensions to each line and then split the spiral into separate parts every 15 degrees.

The problem is that resizing the spiral is an issue… I think that the sectional lines are moving and adjusting as they should when resizing BUT they end up adjusting to where the arc line ends and since the sectional lines are constrained to that arc line, they do not really know what to do when they reach the end of the arc line, and understandably don’t know that I want them to simply expand into the next arc line.

I tried using a spline to have one singular line to constrain all of the lines to but I could not really figure out how to make it work.

I cannot just draw lines over the spiral either… I need to be able to have the spiral in sections. How would you go about dividing it while still being able to adjust its size if you need to?

[etfrench]

If you extrude it first, you can use a separate sketch to split it.  Use formulas to create the split paths, or use pattern on path with a surface to do the splits.