Sketch Origin not aligned to Model origin

[Anonymous]

Hello,

I hope someone can help me, I have created these planes as below by offsets from the origin. I intend to create a loft through the three angled planes.

However when I create a sketch on the left, uppermost angled plane, the sketch origin is not aligned to the model origin, as below. 

I can project up from the model to get the correct centre and continue the drawing. But I would like to know why the sketch centre is not aligned to the origin and if/how to fix it.

Thank you for your time.

[Phil.E]

@Anonymous

Welcome to the Fusion 360 community.

The origin of a new sketch does not always match the model origin. If you were sketching far from the origin it would be of little value to automatically center the sketch on the component origin, far from where you are working. We have gone back and forth on this, and what you are seeing is the result.

It's intentionally this way, but we're open to suggestions. Can you show more of your sketch(es) for the loft so I can understand more of your workflow? I would like to see how you work around this so I can replicate the situation. 

Thanks,

[Anonymous]

Hi Phil,

Thank you very much for your reply. I see, that makes sense if your sketch is far from the origin. Here are the three sketches and the loft, the right hand two reference the centre of the left most circle, which is aligned to the model origin. I couldn't figure out how to remove that edge on lower left of the loft but I guess that is part of the solving/wrapping?

Here is the end sketch and zoom in on the centre to show that the sketch centre and origin centre are very close, 5.281mm apart. I selected the wrong centre many times when both drawing and dimensioning, so I added an extra plane on the front plane that I could extend up through the sketch to help me select the correct centre. Please excuse my drawing technique, I just started using CAD again last week after 10 years absence.

I'll include this final picture for context. Is there no way to move/align the sketch centre? My suggestion would be something like, after I've started drawing, I can set the sketch origin to a point. It is curious though, if all of my previous sketches were using the model centre, why this sketch moved 5.281mm to the side. Thanks again, Thomas

[Phil.E]

@Anonymous Thanks for the detailed reply. Nice design too!

I can see where this is a problem. I'm a little surprised to see such a small difference in the origin. If I could look at the model it would help. Perhaps there is some logic that could prevent this situation.

If you feel comfortable sharing you can post the model here, or I can email you for a link. 

Regards,

[Anonymous]

Hi Phil,

Thank you, it is just a rough model produced from some drawings and photos I was provided with so it's fine to share. Maybe I have done something odd from the start that has followed through.

http://a360.co/2kDe1Vp

Hopefully I have shared that correctly with the right model.

Thanks again.

[Phil.E · Accepted solution]

@Anonymous

Thanks for the model and I can confirm there is nothing you did to cause this. Fusion calculates the sketch origin using a method that does not take into account the model origin entirely. I've logged an improvement request to bring this experience in line with Inventor.

As you can imagine, sketches can show up anywhere, at any angle, on any plane, and it can be tough to always produce the "best" origin location. In this case, when the sketch is centered on the origin and there is no model geometry influencing it (such as a skewed bounding box based on the model), I can't think of why Sketch would place the origin just slightly to one side. It's clearly trying to get the sketch origin close to the model origin.

There is no guarantee this will be taken up any time soon, so for now, pay close attention to sketch origin placement and model accordingly.

(internal reference FUS-37679)

Thanks!

[Anonymous]

Thanks for checking that Phil! You mention a skewed bounding box, is there some way to control the sketch centre with this bounding box?

[Phil.E]

@Anonymous

No, that would not produce anything useful and would likely never be accurate fully. In this case I'd prefer to look at the code and provide more consistent results.

[HughesTooling]

If you create a sketch on a face the origin is always at the component origin but if you create an offset plane from a face the origin will be at the centre of the face. 

@Phil.E Take a look at this thread, personally I'd like the origin to update if the face changes, at the moment it's fixed at the centre of the face when the plane was first created.

Edit, The sketch in the thread above is from a plane created off a plane then an axis then another offset plane so the origin could end up anywhere.

I have another thread here showing a problem with 3 point plane not updating as well.

Here's a screencast showing the difference between sketch on face and using an offset plane. Also notice the odd ghost plane when I drag the offset plane and the offset text origin in the sketches. It looks like the text origin is somehow fixed to the document origin not the sketch origin! My file's attached.

Mark

[ed]

Definitely annoying.  Need an option (checkbox) to use the model origin

[Phil.E]

With the major update this week, the sketch origin should always be the component origin. Can you test it out and let me know if it performs as expected?