Messed up patches due to parameter change

[fritter63]

See attached file. I was finally able to get this modeled with parametric controls. However, note what happens if you change

the parameter "HeelHeight". I oringinally drew it with a height lf 75 mm, then realized it should be 84.5 mm. However, when

you change the parameter to that, although the attached spline and heel cap move as desired, note that the patched surface (body 13) gets seriously screwed up. It's not like it doesn't stretch correct, the of the adjecent edges actually appears to move move on the co-ordinate system.

Is this a bug? Or did I model it incorrectly? What would be the correct way to model this so that the height parameter can be changed and keep the surfaces intact?

Thanks.

[jeff_strater]

I'm looking into this model.  It may take a little bit, so stay tuned...

Jeff Strater (Fusion development)

[gautham_kattethota]

Hi,

The fact that you end up getting a twisted and wierd patch surface after you change the parameter value is not right.  It is a defect and I have reported it to the relevant team.  The problem arises because the boundary edges for the patch get close to tangent as you increase the parameter value.  We should be able to fix this.  Thanks for reporting it.

Regards

Gautham

[jeff_strater]

Thanks, @gautham_kattethota for tracking down the patch bug.

However, looking at your design, I'd like to offer another workflow.  There are a couple of reasons for this.  First, of course, is the patch bug.  The second reason is that Patch tends to be "noisy", and to generate questionable geometry in some cases.  Given the geometry in this case, I would be skeptical of the results.

So, I would suggest using a loft instead, for the whole heel, and overshoot it, then trim it back.  Something like this:

So, I started out with your design, and rolled back before your loft.  Then, I added some geometry to some of your sketches, and created a new sketch:

Then, I created a loft as described above.  The resulting geometry is pretty nice:

Then, using the offset in HeelCap, I just trimmed off the top of the heel:

  

This should result in better geometry, IMO, and should make it more editable via parameters.  If I change the HeelHeight to 84.5, it all updates, but the shape is not quite desirable - we'd have to edit the rail curves a bit to get a better result:

I've attached my version of the design here, as well.

Hope this helps somewhat in your design,

Jeff

[cekuhnen]

@jeff_strater

That way is also I think the proper way to do it. Overbuild and cut is such a common workflow.

[fritter63]

Thanks Jeff, that does look like good way to do it. I didn't realize the loft woud work like that.

A couple questions though:

1) couldn't you skip the extra cut profile and just use the existing heel cap drawing, then select "extend cut surface" on the dialog?

2) the picture you show of the finished heel doesn't match the previous drawings. The heel cap should come to a point in the middle (what is currently the right side)

however in your picture the curve at the heel is quite different. This is crucial actually, as the point looks better.

3) would it be better to make the spline an arc instead? Assuming the profile could be matched, maybe that would adapt to height changes better?

[jeff_strater]

Good points, @fritter63

1. yes, that's a better approach anyway.  Use Split Body, and extend the cut surface.  Great suggestion.

2. also agree.  I was not particularly careful in my geometry, to be honest.  You would probably want to take a bit more time with the geometry

3. another good point.  

Anyway, give this method a shot and see if it can work for you.  Hopefully you will be able to get the results you want

Jeff

[fritter63]

Hey Jeff,

I'm trying to recreate what you did and a few questions/problems.

The arc vs spline does seem to work better when changing the parameter.

However, when I try to specify the arc (formerly the spline on the front of the heel) as a rail, it tells me it is not connected to both the profiles.

When I drew it, I did project/include and selected the centerline from the heel cap end sketch, and snapped to the ends. So I'm not sure why it isn't connected. Do you have to somehow

select the actual surface/body when snapping to it? Can you detail how to go about doing that?

Thanks

[fritter63]

I think the problem is that I have TWO surfaces for one end of the loft, created by adding the top part the end of the heel. What is right way to make it treat this as one profile?

I tried "stitching" them, but it won't even let me select the surfaces when I do that.

[jeff_strater]

A couple of comments:

1. On your second post, you ask about the two surfaces for the end of the loft.  Yes, there are two profiles for that end of the loft, but the loft command should just merge them together for you, because they are in the same sketch, and are coplanar.  So, that takes care of itself.

2.  Below is a screencast of how I did this with your model.  As you can see from the screencast, I had to re-do part of your HeelEnd sketch.  I'm not completely sure why, to be honest.  I have an open question with our modeler team to see why that is the case.  Unless I did that, I got an error saying the loft was "self-intersecting".  I'm not sure why, it sure doesn't look self-intersecting.  And, as near as I can tell, the geometry I replaced it with should be nearly the same.  I do know that loft can be "fiddly" and is picky about the geometry that goes into it.

3.  Another thing you'll notice from the screencast is my use of Project.  Again, loft is picky.  The best way to assure success is to project points from one sketch into the others to make absolutely certain that the points match, especially for rails.

4. For some reason, I had to create the patch surface to use Split Body.  I'm not sure why, I thought it was supposed to work with sketch profiles.  I'll have to look into that one, too.

5.  Finally, for some reason, the loft is sensitive to how high the added top part to HeelEnd is.  I found this by pure trial-and-error.  If I made it too high or pointed, it failed.

I do see what you mean in your point about the heel coming to a point in the middle.  I don't have a good answer on that one.  Perhaps that can be controlled by changing the rail curves, or maybe adding more rail curves.

Anwyay, here is the screencast, sorry it is so long (3:30), but I was going as fast as I could.  Here is the link, also:  http://autode.sk/1L5ytlP

Jeff

[jeff_strater]

One last point:  With lots of help from our modeling kernel guys, we figured out the "self-intersecting loft" problem.  Your original sketch "HeelEnd", has some points that are very close together.  If you zoom into this area:

You will see this:

When I created the rail for that side, I suspect I projected the wrong point, so the rail did not attach right at the corner of the profile.  This causes the loft to fail.  So, again, you have to be really careful when setting up rail curves that you get the exact right point.

So, anyway, I probably didn't need to reconstruct that portion of that sketch, just be a bit more careful when creating the side rails.  My error...

Jeff

[fritter63]

OK, I've played around with it some using your approach and I'm still have some issues. See attached design file.

I've switched the splines for the main curves (the ones I want to keep in the shape) to be conic curves rather than splines. I was still

able to get the curves I wanted with fewer points.

However, when I try to loft now, using only the spline as a rail, I get the G1 error (not smooth). I've adjusted it as much as I can and it looks

pretty darn smooth to me between the two sections. I see that there is a "smooth" constraint, is that meant to correct this situation? I can't 

figure out how to use the thing.

Also, is there a doc page somewhere that explains what different symbols mean in the UI? Ie, when points are colored and there are different other

"looks" I can see and it's not clear what they mean. I haven't seen a good explanation of that anywhere. Is "red" just locked? Or does it also mean projected?

I'm seeing an issue where when I try to select the rail with "chaining", it actually gets the extension line from the HeelEnd sketch as well! I can turn off chaining, but how

then do you select both curves for the rail without getting the intersection error message?

Also, what does "closed" mean (checkbox) when doing the loft? If I look it up in the learning center, it will likely say "switches to close/unclosed". Docs like that don't help!

Why do some of my designs show with red backgrounds on the left panel?

One last comment, getting up on my soapbox now. The UI for these operations (lofting) are just too **** picky. The point of a UI is to make it EASY to do these complex things, and I 

think Fusion has missed the mark on this particular operation (most of Fusion is pretty easy to use though). If I have to spend literally hours just fussing to get things just right to make

it happy, then the software is not robust enough. Why should it matter if the rails are smooth? Who cares if the extended rail is too high? Run the **** calcs and follow the lines. At this point it would have been faster for me program the shape in Python or JavaScript then trying to make the UI happy. 

</soapbox>

[jeff_strater · Accepted solution]

Thanks, @fritter63.

I can answer some of your questions.  I'll start with the one I can't answer:  I don't know, honestly, if there is any single place where all of the colors and symbols are documented.  Such a thing would be useful, I agree.  Maybe others here can point to where this may be documented.

Now, on to your specific loft issues.  I see two problems with your design.  One is related to the issue that I also ran into.  The profile in the HeelEnd sketch has those two points that are very close together.  And this plays lots of havoc with the loft, because the rail curve is not hitting the true corner of the profile.  Here is a very zoomed-in view of that area in the latest model you shared:

You can also see this if you do a Measure and select the workplane at the top and the side face of the neck:

You can see that they are 0.023mm apart.  That plane is related to that vertical line in HeelEnd.

For that one, I had to edit HeelEnd and force those two points to be coincident.

The second problem was the one the command was telling you about:  Your rail is not tangent (G1) continuous.  That one was easier to fix.  Just edit the HeelSpline sketch, and add a tangent constraint.

With those two edits, I was able to create the loft.  However, the resulting geometry is probably not ideal.  You may need to make some tweaks to profile curves, rail curves, etc to get the desired geometry.  You can also edit the loft and change the "point mapping" (each point on a profile must be mapped to a point on the next profile).  This shows up as lines in the preview that can be dragged.

Here is another screencast showing how I edited your design to get it to work:

 "closed" in Loft is used if you want to create a loft that closes in on itself.  For instance, if you have these 4 circular profiles:

And you create a loft, and select all 4, you get this:

If you check the "closed" option, it creates a closed loft:

Next, Chaining during rail selection.  If you turn off chaining, then you should be able to select curves piecewise, and If they are connected, Fusion will recognize them as the same chain, and string them together.

Red backgrounds in the data panel.  This is a bug, that there is a fix for, but hasn't made it to a release yet.

"picky" UI.  I understand the frustration.  Loft is a complex operation.  The underlying math is complex as well, and dictates many of the requirements that show themselves in the UI (for instance, the G1 tangent requirement, the requirement that the rails must exactly intersect the profiles, etc).  You could argue that the software is bad, and certainly it could be improved (what software could not use some improvement?).  However, to be frank, it's not quite as easy as it may seem.  I suspect that you will find that any CAD package that supports Loft will have many of the same limitations.

Jeff

[fritter63]

ok, thanks for the replies Jeff.

Interesting about those two points.... that vertical line should have started at the same location as the horizontal "neck surface" line. I'll have to see why that is like that.

[fritter63]

@jeff_strater

Ok, I played around with it a bit late last night... and I think I see the root of the problem.

The reference plane I made for the spline was based on the inside edge (that line that will get mirrored for the complete neck) of the heel cap geometry, and

that line was somehow off by that set distance (0.023 mm?) from the "centerline" (right edge in this case) of the eventual neck.

So when I did "reference plane at an angle" to that line, the plane for the spline is off. WHen I did project/include

of the points through that sketch/plane, it created that point on the plane, and then the spline would snap to that point, looking like it was in the right place, but actually

doesn't tough the neck surface on the other end of the spline. Hence the "not connected errors" I was getting.

I guess project/intersect would have solved that and made it obvious I had a problem?

Will report once I've fixed those. Was too late last night and I kept messing it up.