Angled Sketch Plane Dimensions Wrong. Why?

[glencandle]

I've searched this problem first but I can't find a solution.  Basically when I create a sketch plane with an offset angle of 10-degrees, then draw a sketch on it, the math for the drawing doesn't work out.  

When I'm drawing my sketch I'm making a rectangle that is exactly 33" x 45" along X,Y.  Yet when I use the Dimension tool and measure the drawing I get 33.104" x 44.923".

I'm sure this is because of the angle of the sketch plane (10-degrees), but I have no idea how to get around this.  I need this part, despite the angle, to exactly 33x45.  What do I do?

[g-andresen]

Hi,

Please share the file for investigation.

File > export > save as f3d on local drive  > attach it to the next post.

günther

[glencandle]

Hi Gunther, thanks for your response.  Here is the file you requested:

https://www.dropbox.com/s/k9yzkbf0fqtpxwu/Dimension%20Error.f3d?dl=0 

[TheCADWhisperer]

@glencandle 

Are there any unresolved issues highlighted in your timeline?

Does Ctrl b on Windows or CMD b on Mac return any errors?

Is your geometry located relative to the Origin utilizing obvious symmetry?

What happens if you start over from scratch in a new file?

[TheCADWhisperer]

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@glencandle wrote:

Basically when I create a sketch plane with an offset angle of 10-degrees,  

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@glencandle 

There is no reference for the  10°plane in the file that you linked.

Did you delete the plane?

I assume you deleted some reference that is shown ghosted in your original image.

See Attached file below.  (When you open it in Fusion it might be on the second tab rather than the first tab.)

[glencandle]

Hi, sorry about that. I cleaned up my project file but I went too far.  The attached project file is the corrected one.  The sketch in question is in Component 2 called "Sketch With Issue" and the sketch plane it is attached to is called "Angled Plane" (also in Component 2).

Thanks!

[glencandle]

Hi, just checking in to see if anyone has had a chance to check this out yet?  I would love to know what's going on here, thanks.

[davebYYPCU]

Well, only way to describe it, sloppy sketching.

Near the left vertical line is another (short one circled) construction line, that is not vertical, the end point is 16.5 from the side measured - vertically.  The centre line is perpendicular to the short line, but not horizontal!

This angle makes the other side line longer than 33mm.

Odd angles everywhere.

Might help.....

[glencandle]

Hey @davebYYPCU thanks for taking a look at this, I really appreciate it. 

However, I reject your claim that this is "sloppy sketching" (lol!).  All I did was project the geometry underneath (which is entirely straight) onto this plane to find the center point; and then used that point as a reference for my sketch.  All of my lines were drawn straight, manually sized (as you can see, 45", and 16.5"*2), but after creating them, and using the dimension tool, the measurements are incorrect.

Sloppy sketching aside, can you explain to me how the line I drew says 45" where I drew it, but 44.923" where the dimension tool has measured it?  How does that make sense, exactly? 

[davebYYPCU]

Then tell me why this is not sloppy.

Delete these two lines (selecting near the crosses)

Your 45mm centre line is NOT horizontal.

The 2 short vertical construction lines are NOT vertical.

This results in a layout of a Z (zed) that makes the outside horizontal lines shorter than 45mm

To fix it delete all the perpendicular and midpoint constraints, (all of these, or you will hit more errors)

Now add vertical constraints to the short construction lines, Perpendicular the centre line at one end, and coincident the centre line with the centre point of the construction line (sorta) square.

Extend the short construction lines to the outside corner and make both end points coincident.  Your outside rectangle is no longer a parallelogram.

I am not fixing the internal shape unless you get stuck.  (I need to know the length of the sides)

PS.  That square is not a square as it has 4 different corner angles, and four different side lengths.

PPS Would have been real easy to draw a 2 point rectangle and set the dimensions, for placement.

Might help....

[glencandle]

I agree with @davebYYPCU that the outcome is sloppy. However, none of the issues you're pointing out were sketched that way, those are the outcomes of whatever glitch is at work here.  When I drew this sketch I was drawing perfectly horizontal and vertical lines, there should be no angles.  This is what I'm trying to figure out.

Can you please address the simple question of how a drawn line with the length of 45" (manually inserted) can thusly measure out to be less than that?  I would very much like to know how this can be.  

Other than the fact that Fusion 360 is measuring the distance from the perspective of the camera, which, considering the 10º angle of the sketch plane, would indeed make a shorter length.  But everything I have read about Fusion says that it doesn't work that way.  It should be measuring the actual dimension of the sketch along its local axis, not from the perspective of the camera looking down Z.  This is the heart of my confusion, again, how a line that is 45" can measure out to be less than that.

In my limited experience with Fusion, a dimension manually input is a fixed dimension, no?

[jeff_strater]

"Can you please address the simple question of how a drawn line with the length of 45" (manually inserted) can thusly measure out to be less than that?  I would very much like to know how this can be.  "

@davebYYPCU is correct - the problem is the sketch itself.  The 45 inch dimension is not between the same geometry that the driven dimension is measuring.  There is a small construction line which is not constrained to be horizontal.  You can see this in a number of ways using Measure:

you can see that these two lines are at an angle if you zoom in close:

you can also see this if you measure the angle to the vertical line:

the angle is small, but .13 degrees is enough to make the difference between what you see in the driven and driving dimensions.

[davebYYPCU]

I have exaggerated your construction, 

Your 45mm centre line only when vertical, will keep the outside lines 45mm long, , but it was never vertical or horizontal which ever way you look at the sketch.  However the outside driven dimensions are paired, as expected.

Might help.....

[glencandle]

Hi Jeff, thanks for your input. 

I guess the confusion here, at least for me, is that I did not sketch these lines at an angle.  That is the outcome of whatever happened to my sketch after I drew it.  Or so it seems at least from my perspective. 

You're seeing the end-result of the sketch, but my thing is that I drew straight lines and they came out inaccurate, for whatever reason. 

I'm assuming this is because of the angle of the sketch plane, but again, I am under the belief that the angle of a sketch plane should not skew the dimensions of my drawing.  Maybe I'm wrong?

[davebYYPCU]

Has nothing to do with the plane at Angle!  It was user error!

The external rectangle was constrained on all four sides to be horizontal and vertical respectively, on that plane.

For some reason it went astray, User error, when the 3 construction lines were not vertical and horizontal, but own the dimensions.  

Fusion has correctly reported to you, that this small angle makes the long sides of the rectangle short, and short sides longer, because the construction lines are at a small angle, relative to the rectangle.  There is no glitch coming from Fusion, it was your non constrained construction lines that are doing as told.

Another way to fix this, delete the construction lines, and dimension the outside rectangle, when that is done, constrain the rectangle where you want it to be.  

Same for the inside shape, (an even worse mess - 4 sided polygon) it appears you delete automatic (very helpful) constraints, and draw lines nearly right, complain that Fusion got it wrong.  

Totally user input that gets it in the state you delivered the file to us in.

Might help....

[jeff_strater]

As there is no history captured for a sketch, it is a little hard to say what might have happened along the way.  All I can see from the current state is:  That construction line does not have a Horizontal constraint on it, which is what would have prevented it from deviating from horizontal.  Many things might have caused that line to rotate - an inadvertent drag, a dimension to the endpoint instead of the line, etc.

I have never seen any cases where the angle of the plane with respect to a component or global coordinate system has caused geometry to misbehave.  That is not to say it is impossible, I just have never seen it.  Each sketch has its own coordinate system that it uses within the sketch.  That coordinate system is oriented so that the Z axis is normal to the sketch plane.  If you stick to pure 2D sketching, sketch coordinates will all contain values only for X and Y.  So, in theory, that plane could rotate in any direction, and the sketch should behave correctly, independently of the angle of the plane.

[davebYYPCU · Accepted solution]

What I would do, needs one more dimension, because you gave me a choice of 2, will let you decide, where to put it.

Might help....

[glencandle]

Thank you @jeff_strater and @davebYYPCU for your help, I really appreciate your time.  Perhaps this is a product of bad form, haha, but honestly I've been using Fusion for a few years now and I've never had this issue, nor any 'sloppy sketching' accusations 😉

I didn't want to make my design public so I tried to clean up as much as possible and still preserve the issue, but I think I didn't do this cleanly enough and what you're seeing just appears to be a big mess. 

My theory about what happened is that I projected the underneath geometry onto the plane, but because the plane was at a 10-degree angle the geometry was projected with perspective instead of orthographically (which is probably my bad), though there is a very good chance I'm wrong there!

I thank you again for your help, I learned a lot 🙂

[jeff_strater]

"but because the plane was at a 10-degree angle the geometry was projected with perspective instead of orthographically"

I can verify that this does not happen.  All projections happen orthographically, regardless of the view mode.  However...   There are cases where the sketch coordinate system can get slightly rotated with respect to the global coordinate system.  So, it could be that this might be the case, and projecting a model edge at a slight angle with respect to the sketch coordinate system.  I don't think that this is happening in your design, but because this is a subset, it is hard to say whether that is the case.

[davebYYPCU]

When you check my file, the 2 purple projected lines are as you would expect, not the same length as the original, simple and plain logic, due to the Plane at an Angle.

For them to be the same length you have to Copy / Paste them.

Might help....