Best way to move (rotate) for .001mm movement.

[CB63]

Hello Forum,

I've been playing around with an airfoil generator which seems to work pretty good so far. I've run into a problem on positioning the sketch, straight and true, along the Y-axis.

While I do realize that I'm not building a stealth aircraft to protect the United States interests I would like "true up"the position of the airfoil. I've included three screencaps that show:

Point A along the Y-axis and

Point B along the Y-axis (+.001mm)

I've tried several iterations of pivot points, etc. but I am unable to get a perfectly level wing chord. Any takers? I appreciate your time in viewing this and welcome any suggestions.

[laughingcreek]

Ok, you asked for suggestions.

First suggestion. realize that .001 mm is so far outside the range of tolerance for any method your likely to employ to make this thing, that it's not worth another second of your time to fight it.

second suggestion.  keep in mind that those wonderful ,exacting curves, generated by the airfoil generator has been sliced and diced, and generally turned into garbage by fusion when you imported them.   I'm guessing you are about to make a wing from this profile, so lofting is in your future.  These minced up curves are going to give you a head ache at some point, because they frequently don't play well with loft.  Usual work flow is to rebuild imported curves with native fusion curves.  this will probably introduce errors in access of .001 mm, but you can get it close enough to not matter. (wish fusion had a "match curves" tool for rebuilding curves. maybe someday)

[laughingcreek]

you can also draw a horizontal line and measure the angle between the to.  then use move to rotate that amount.  set your pivot point so it's rotating from point a.  and you'll have to adjust your precision and display settings for units in "preferences" to get it to show you such a small angle.

[CB63]

Self solved.

By selecting the move command and positioning the point as shown in this screencap I was then able to select a value of -.001 at that position and the sketch only moved (pivoted) at this end.

I'm not for sure why I now get a value of 4.778E-05 mm for Position Y but it appears to have worked. Thanks Alex for taking the time to look at this and offering up a solution.

[n8bot]

While it might seem like you have achieved what you want, I suggest doing a few things. First, add some constraints to the sketch to fix it in place. Perhaps dimension some curves (if those are curves) or simply fix some things in place. For the trailing edge, I suggest you fix that point to the midpoint of the line it resides on, and then put a horizontal constraint between that point and the point on the leading edge (which you will have constrained to be fixed on that curve beforehand).

[TrippyLighting]

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@laughingcreek wrote:

Ok, you asked for suggestions.

First suggestion. realize that .001 mm is so far outside the range of tolerance for any method your likely to employ to make this thing, that it's not worth another second of your time to fight it.

second suggestion.  keep in mind that those wonderful ,exacting curves, generated by the airfoil generator has been sliced and diced, and generally turned into garbage by fusion when you imported them.   I'm guessing you are about to make a wing from this profile, so lofting is in your future.  These minced up curves are going to give you a head ache at some point, because they frequently don't play well with loft.  Usual work flow is to rebuild imported curves with native fusion curves.  this will probably introduce errors in access of .001 mm, but you can get it close enough to not matter. (wish fusion had a "match curves" tool for rebuilding curves. maybe someday)

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@CB63 This is spot on advice and I've got noting to add other than you should be  listening to it. 

[CB63]

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@TrippyLighting wrote:

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@laughingcreek wrote:

Ok, you asked for suggestions.

First suggestion. realize that .001 mm is so far outside the range of tolerance for any method your likely to employ to make this thing, that it's not worth another second of your time to fight it.

second suggestion.  keep in mind that those wonderful ,exacting curves, generated by the airfoil generator has been sliced and diced, and generally turned into garbage by fusion when you imported them.   I'm guessing you are about to make a wing from this profile, so lofting is in your future.  These minced up curves are going to give you a head ache at some point, because they frequently don't play well with loft.  Usual work flow is to rebuild imported curves with native fusion curves.  this will probably introduce errors in access of .001 mm, but you can get it close enough to not matter. (wish fusion had a "match curves" tool for rebuilding curves. maybe someday)

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@CB63 This is spot on advice and I've got noting to add other than you should be  listening to it. 

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I realize now that I'm splitting hairs, so to speak but it does present a challenge. It would be nice if Fusion did have a match curves tool for rebuilding curves. Good advice all around as usual from the forum participants.

Thanks again.

[etfrench]

It does have curve matching if you're willing to do a few extra steps.

[CB63]

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@etfrench wrote:

It does have curve matching if you're willing to do a few extra steps.

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Wow! I gotta let that procedure sink in for a bit.

Thanks.

[laughingcreek]

yes, the mesh cross section matching  work around,(and the t-spline work around) is a was to get matching functionality.  But I mean really, explaining the whole-extrude, convert to mesh, get a cross section, match the cross section--routine is a bit tiresome.  And would really rather not have the extra stuff in my own designs.  Converting to a mesh first can also add more error to the curve before even starting the match process. (the mesh itself is jut an approximation).  Would be nice to be able to use the that matching tool directly on a curve.

[TrippyLighting]

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@laughingcreek wrote:

  Would be nice to be able to use the that matching tool directly on a curve.

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Yes, there are a number of tools burried in some parts of Fusion 360 that would be useful as a general modeling toosl. This is one example, the sheet metal environment is another example.

[etfrench]

After creating the new profile,  you may be able to align it to any arbitrary position. 

• Sketch should be in a component.
• In the sketch draw a line between the end points (or the points you want aligned).
• Extrude the geometry a short negative distance.
• Create a Joint Origin at the midpoint of the line (if necessary).
• In a separate sketch in a new component, create a line.
• Use a Rigid joint to align the first sketch extruded geometry with the new position line.

Theoretically, the geometry and its sketch should be perfectly aligned with the new position line.