How to move fixed geometry into sketch origin?

[prscustom]

I just want to constrain the center of the circle with sketch origin. It needs to stay fixed.

[TheCADWhisperer]

I recommend that you start over from scratch and this time sketch your circle at the Origin.

When you reproduce the sketch - be sure to fully dimension/constrain each and every bit of geometry including the spline handles.  That way anyone can reproduce the geometry (and at any location).

[TheCADWhisperer]

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@prscustom wrote:

Thanks for the effort but no, its not acceptable.  And there should be no need to change because theres nothing wrong with the sketch.

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This image is from your original problem description.

This is not the same sketch as the file that you Attached.

I would have preferred to have the sketch in this condition from the original problem description rather than as in the file that you attached.

[prscustom]

Ok, here you go

[TheCADWhisperer]

I haven't checked your latest attachment yet, but how about this one?

Now I will go check your latest attachment.

[jeff_strater]

@prscustom - the problem (it may be obvious, but IMO worth pointing out), is this point in the upper spline:

It seems to be "locked" for movement, no matter what I do.  Even if I delete the coincident constraint, and move the circle away from it:

I cannot move this point - either by dragging or with Move.  It is not locked, and appears to have no constraints on it.  So, that is the root cause of the problem here.  If I delete that spline and re-create it, everything moves just fine.

So, the question to you is:  Do you have any recollection of how that spline, and particularly that point was created that might have caused this?  Any constraints that existed in the past?  

I'll continue to look into this as I have time.  Something weird is going on, definitely

[jeff_strater]

OK, found out some more.  It seems that point cannot move because its tangent handle (line + both endpoints) are also locked.  So, unlocking those will allow the sketch to move.

However, this does perturb the spline.  For that, I will have to go to the sketch team to investigate it.  I'm not sure what is causing that.  Possibly unlocking the tangent handle?

[TrippyLighting]

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@jeff_strater wrote:

@prscustom - the problem (it may be obvious, but IMO worth pointing out), is this point in the upper spline:

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Yep, that is exactly what I've observed as well. I've seen this only once in another users design and it's quite a while back. It was also a spline point that I could not move by any means. 

IIRC some time during the design process the Fix constraint had been applied in that design as well, so I am wondering if that is the root cause in this case.

[jeff_strater]

@prscustom  - just a follow up:  The sketch team is going to look at two issues:

1. the shape change on move after unfixing the tangent handle - this is unexpected, I believe
2. we will discuss some UI changes to better indicate the condition here:  A fixed tangent handle that is not shown.  Not sure yet what we will do to show this, but hopefully we can find some way...

[TheCADWhisperer]

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@jeff_strater wrote:

…but hopefully we can find some way...

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You could “walk” across the hall and ask your Inventor Professional teammates how to do Sketch Blocks.  Might help!

[prscustom]

Thanks for the reply and i hope it will be fixed, although i doubt it will

Bcs meanwhile i've encountered another dealbreaking problem and there are many posts about this exact same problem dating years back and appearantly still hasnt been fixed.

Projected lines dont close in sketch, so i cant do anything (like a simple extrude) with them. I dont understand how something so simple and essential can fail, but there it is.

Exact same operation works in other cads ofc, like Inventor, even when i export the body in IGES. (Also for some reason i cant export .ipt anymore?