Can't get hole to move

[matthewrjacobs]

I'm trying to get the bottom set of holes (see screenshot below) to move up a mm or so,  but no matter what I do I can't get them to move.

The holes are at a 6deg angle, I created them by drawing circle, a construction plane, then drawing a line at the angle I wanted on the plane,  then did a cut sweep along the line, and patterned the rest of the holes of of that.   I can change the angle of line which puts the exit of hole where I want it, but not the entry of the hole.  Maybe there is a constraint locking it there but I can't seem to get rid of it.

the top set of holes is fine

[laughingcreek · Accepted solution]

The center of the circle in sketch 36 is constrained to the end point of a line from sketch 35 that has been projected into the sketch-

after deleting the coincident constraint-

you can't see the constraint in sketch 36 till you turn off the visibility of sketch 35.  I think this is because  the profile (the light blue area of a closed loop in a sketch) is interfering with it.  simply  turning off visibility of profiles in sketch 35 should have solved that problem, but you have "auto project geometry onto active sketch plane" checked on in your preferences (go turn that off now).  when you create a sketch on the face of a body, it will "project" the edges of the body into the sketch.  the catch is these projected edges are invisible (so as not to clutter up the sketch, I was told with a straight face).  these edges form a profile who's visibility aren't controlled by the "show profile" visibility checkbox.  deleting some of the edges also doesn't get rid of the profile.

The result is you can't see the constrain glif when sketch that has projected from visible.

seems like several bugs at play here.

[matthewrjacobs]

@laughingcreek If by bugs, you mean my hack design flow,  I agree!  

I followed your advice and was able to delete the coincidence.  Thank you.

I did notice another problem I can't get rid of.  There is a half circle (face?) covering the hole.  It wasn't there when I created the hole and doesn't extrude through.   but I can't delete it,  it also happens to be on the construction plane, which has a bunch of projection garbage going on in the area. 

Any suggestions?

[laughingcreek]

The half face seems to be related to the construction plane yourusing for the sweep line.  it's hard to say why.  The whole body is in an error state and your working off cached geometry.

this can lead to a whole host of unpredictable weirdness.  You will be chasing your tail trying to figure out what is wrong with that hole till the error gets fixed. 

FYI-I guess you realize that sweeping a circle at an angle produces an oval shaped hole, not a circular one?  IDK, maybe that's intended.

you asked for a suggestion.  mine would be to start over.

in a new model-

1-create a new component, make sure it's activated.

2-create a sketch on the YZ origin plane.

3-draw and fully constrain this cross section shown here-

have the origin of the sketch be on 1 of the 3 points shown along bottom edge.  my preference would be the midpoint.

4-come back here and post the .f3d of just that.

you should be able to do what you've got so far with 3 or 4 sketches and a handful of features.

(any ref pics/drawings your working from would be helpful also)

[matthew.jacobsNTYPH]

@laughingcreek   Thanks for the feedback, see my comments below in blue 

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@laughingcreek wrote:

FYI-I guess you realize that sweeping a circle at an angle produces an oval shaped hole, not a circular one?  IDK, maybe that's intended.  yes,  but it needs to be at an angle so the holes exit in the right place

you asked for a suggestion.  mine would be to start over.

in a new model-

1-create a new component, make sure it's activated.

2-create a sketch on the YZ origin plane.

3-draw and fully constrain this cross section shown here-

have the origin of the sketch be on 1 of the 3 points shown along bottom edge.  my preference would be the midpoint.

4-come back here and post the .f3d of just that.

you should be able to do what you've got so far with 3 or 4 sketches and a handful of features.

Most of the extraneous sketches, projections, patches are there for toolpath containment, some were successful, some weren't.  I've got the model and toolpaths where it does what I want it to do, so I probably won't start over  anytime soon,  though I may do it just for practice, I'll be sure to reference your advice.

(any ref pics/drawings your working from would be helpful also) 

I don't have any reference other than pics my guitars,  but I've been using more or less the same dimensions for 11 years,  I just transferred them from my noodle to the drawing.  I'd be happy to upload some pics if you want.

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[laughingcreek]

I revisited the hole being half covered.  don't suppose at some point you used the "move" command on that circle?  it's been rotated off plane by an infinitesimal amount.  delete the circle and redraw and it will sweep with out being half covered by a surface.

yeah, I got that the hole needs to be at angle.  but the sweep is at an angle to the circle profile, so the cross section of that channel will be an oval, not a circle.  probably moot since that will probably be cleared with a drill bit.  the angle is so slight that it's hardly noticeable.  but you can't pull a diameter directly off the solid body by clicking the inside face since fusion won't register it as a cylinder.  not a big deal if everything is kept in house.  if you pass the body off to a machinist they'll be calling you for that hole size.  there are of course ways to have that hole be round and at an angle, which is what I was getting at.

[matthew.jacobsNTYPH]

Thanks,  I'll try to redraw when I get home.

you're right, I'm just going to drill the holes, so concentricity of the hole or channel was never a concern.  Honestly I'll drill the holes on a drill press, it's quicker then setting everything up in the CNC.

I'm curious what techniques would make a round hole and a round channel?   or is it a case of one or the other?

[laughingcreek]

assuming you always want a round channel, the mouth of the hole is only  round when the channel is perpendicular to the face.