How to move a feature once constrained?

[Torquindsl]

I know this should be simple, but so far it has eluded me, even after searching this site and the internet. I created a sketch on a flange feature of my project and put construction lines on center in X and Y. Then I created some circles to be made into holes, in symmetry off the center line. I found out after this creation that I put the holes in the wrong place. Now I can't move the holes, I suppose because it is constrained. I have tried, and it goes through the motions to give me a way to move the hole, but when I click OK the hole doesn't actually move and it does not give me any error.

I put a dimension on the hole, from the edge, and it is a driven dimension, so I tried to toggle it to a driving dimension, but it gave me an error. I don't know where the driving dimension or constraint is. It looks like there is a line that the hole is centered on, in the Y axis, but I cannot select that line to move it (hoping the hole/circle will follow).

My problems are:

1. How do I find the constraints to delete them, if necessary, so I can move the hole?

2. How do I move the hole?

Of course, I can "undo" to where I created the holes, but I am trying to learn how to fix mistakes without having to go back a bunch of steps.

I am fine with moving the holes in towards the center line a little ways. They are just for spot welds.

Thanks,

Chris

[TheCADWhisperer]

@Torquindsl 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Click on the center of the circle. 
Does the glyph for Coincident constraint appear?

From the image it appears to be constrained on a Projected line.

You could also delete the projected line if it is not used for anything else.

I suspect that you have Autoproject enabled in your Preferences - most experts here turn that off and take explicit control only Projecting what they need.

[Torquindsl]

The hole/circle I am trying to move is the upper left one on the side is what I have been trying to move.

Thanks,

Chris

[jhackney1972 · Accepted solution]

The video will show you are fighting a Reference (purple) line which cannot be moved.  In the video I will show how to remove the reference status so it can be constrained and dimension.  Model is attached.

[Torquindsl]

Thanks for the info. Did I somehow create the reference line? I don't recall doing so. My process was to create that first hole, then mirror it on the X center line to make the bottom hole, then mirror both holes on the Y center line to create the holes on the right side of that panel. Once I completed that I went o extrude the circles to create the holes and realized my top holes would be behind a flange I created to make a hem on the top edge of the side wall (to make the edge blunt).

I was then going to try to project those four holes to the other side, trying to follow a Lars video, https://www.youtube.com/watch?v=1tURmm-Ywdg

Shouldn't I be able to reposition a reference line, if it is not a center line?

Thanks,

Chris

[jhackney1972]

Reference lines are usually Projected from some other feature so that they will update (move) to reflect changes in the other feature.  I have no idea how your created the reference line.  If you use the Project command and leave the Projection Line checked, the project line will be a Reference line (normal practice).

Center lines can be moved, if they are not constrained or dimensioned but you cannot move a Reference line unless, as I showed you, the link is broken.

As far as the four holes being projected to the other side, you want the projected sketch to be reference circles, then if you change anything about the holes, position or size on the original side, the other side will update.  You also could simply extrude the holes "all the way through" the model and skip the extra sketch.  There are many ways to "skin the cat" as they say.

[TheCADWhisperer]

It appears that you have Projected this edge into your sketch...

...or as noted in earlier response - Fusion might have autoprojected that edge when you clicked to place that circle.

Most experts want explicit control of Projections and turn this off.

[Torquindsl]

Well, I am far from an expert, so do not yet understand the value of this option one way or the other. I will do some searching in the documentation to see if I can get an explanation of the use of this option.

Things are looking good though, for my design. I believe I have it completed, as far as the dimensions and features. I still need to make a flat pattern and get it to something the plasma table will cut.

The spot weld holes are on the inside, so they will not be exposed on the outside, and I got my drawer pull holes in place. There are flanges on the top edges to provide hems (safety edges, if you like), although I could not make those edges 180 degrees because the software did not like that. At 140 degrees it does not complain. Doesn't matter, I know those have to be bent into hems.

Thanks for the assistance.

Chris

[jhackney1972]

For the Hemmed edges, try an angle of 179.9, to make it look realistic.

[Torquindsl]

When I created them I tried various angles from 179 to 140, and it only stopped complaining at 150. Probably something else I am doing wrong, but I have not figured it out yet.

I am going to start a new design to play with that and see if I can make that reference line appear, so I can figure out what causes it.

Thanks,

Chris

[TheCADWhisperer]

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@Torquindsl wrote:

Well, I am far from an expert, so do not yet understand the value of this option one way or the other. I will do some searching in the documentation to see if I can get an explanation of the use of this option.

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@Torquindsl 

Turn it off.

It will just get in the way.

[Torquindsl]

And now it gets weird. I created a new design, just for testing. I created a hem on one side, making it symmetrical so I could narrow the flange a little, to give clearance for the  hem to go on the end flange. Worked out well, no complaints about the angles, unlike my previous design.

But, then I put the same flange on the other side, except I forgot and left it Full Edge. F360 created it and didn't complain at all, even though it clearly interferes with the end flange. Now I wonder why it complains sometimes.

See attached.

Thanks,

Chris