LOFT BUG

[Anonymous]

Hi, my name is Cole and I have only been using Fusion for about 4 months tops. I am still very new but have had a lot of success, except for one model. I was modeling a sword from the game Destiny 2 to be printed, I was trying to loft a quarter of the blade, so i could copy it in a pattern later. I have the two farces and a guide rail, but it is giving me the error, "Wire has self-intersection". I have looked everywhere but there has been no posts for this exact problem. I really need to get this done quick before I lose interest and waste all my hard work. I will attach the file and hope that someone can give me instructions or a tutorial so I can learn from it and avoid the problem with later projects. I have never posted a file so I hope this works, but if anyone can help, it would be greatly appreciated.

[etfrench]

First, read Rule #1.  It will save you much time and grief later

Is this what you're trying to do?

Note: I didn't make any changes to your file before the screencast.

[Anonymous]

I am trying to loft those two objects, but I am trying to use a guide rail that is right above the holy that is connected to the two pieces that you lofted.

[Anonymous]

Holy change to "hilt" and I am trying to give the sword a curved loft instead of a straight triangle type loft.

[etfrench]

I'm not understanding what you're wanting to loft.  Can you make a screencast showing what you're trying to do?

[Anonymous]

I cannot right now, I can tomorrow afternoon, but I will try to explain again. The big, long face and the skinny long face, I want to loft. When you do the loft, it is a straight edge to edge, shortest distance situation. What I want to do, is use a guide rail when I loft so I can have a curve in the loft. The guide rail I want it to follow, is attached to the end of both the faces mentioned before. You are lofting the faces the way I want them to be, I just want the loft to have a curve, rather than a closet distance between to points. Hope this helps and thank you for helping me even if it doesn't get solved, I appreciate it greatly.

[SaeedHamza]

Hi,

It would be much better if you could attach a picture of the final result

---

@Anonymous wrote:
I just want the loft to have a curve, rather than a closet distance between to points

---

This is what happens when the loft have only 2 profiles, you get sharp edges instead of the smooth or curved edges your looking for

[etfrench]

Here's an almost solution.  It worked once (See Sword_02 attached file)

However, when I tried to reproduce it in a screencast, it failed (See Sword_01):

The basic idea is to put the rails and the tip of the sword in separate sketches to make it easier to select the individual rails and the point.

@jeff_strater: Can you take a look at this to see where it's going wrong?

[Anonymous]

I will look at the two files this afternoon but the picture you attached, is exactly what I am trying to do.

[Anonymous]

I just looked at the 2nd file you attached. The one where the blade is lofted. Is it possible for me to drag and drop it from 1 File to another? Just so I can have a reference and the actual building block if anything were to happen?

[beresfordromeo]

Hi

I don't know if this helps but you can also use the patch environment to do what you are trying to do.

I have recorded a screencast for you as a demonstration but I haven't used screencast before so I hope you can see it. 

Basically I opened the sketch of your top profile (sketch 18) and made the spline at the end of your straight line tangent to the line. I then extruded sketches 18 and 20. I placed another straight line on sketch 20 tangent to the sketch 20 spline and used a sweep to make another surface along the path of sketch 16. 

I switched to the patch environment and patched (using tangent (G1)) continuity. Remember to hide sketches and turn off chaining to avoid frustration. What all this does is to instruct Fusion to build a surface tangent to all of the surrounding surface bodies which is pretty much the same a lofting but without some of the possible lofting peculiarities. The loft tool has been called picky by some (even advanced) users and I am inclined to agree with this.

Anyway once you have done the patch you can hide the redundant surfaces, mirror the quarters, close the body and stitch it all together to form a solid body or if you are feeling like pushing yourself a little try using a boundary fill to create the actual body you want.

I hope this helps to get Crown Splitter to market.

 Hmmm can't work out how to embed the screencast. Can anyone give me pointers.

[beresfordromeo]

https://knowledge.autodesk.com/community/screencast/7cc22cac-7e46-4f01-a651-87625a3c2709

[beresfordromeo]

Ah ok, you cannot insert a screencast in an edit maybe. Anyway sorry for messing up this thread.

[etfrench]

You can copy and paste between open files.  In this case I wouldn't recommend it as you will have to rebuild the references.  I will recommend that you start this project with a new file and follow Rule #1.  The contents of sketches 16, 18, and 20 can be copied into new sketches.  The sketches used to create the hilt can be copied in the same manner.

[beresfordromeo]

Hi etfrench

I don't mean to be disagreeable but I don't think that there is any need for a restart. I went through the file and rectified the sketch warnings. Mostly they just needed the sketch plane redefined but sketch 20 had actually lost a plane I think. All I had to do was go back in the timeline, create a 'plane at angle' from the horizontal line on sketch 16. then 'redefine sketch plane' of sketch 20 to that plane.  I then did the same as you, mirrored the spline etc. on sketch 20 and the loft that you were attempting then worked.

That was an interesting loft and not one I have considered before so thanks for your video. I think though that I understand why your loft didn't work. To put it simply, I think it is because you needed to close out the top profile of sketch 18 (in the original model). This allows for a profile to point loft as you did with four guide rails... as long as tangent chain is switched off.

When you select rail 1 in your video at 3:21, tangent chain is on which I found led to some problems, I don't think this is a problem in your sketch because you have no other tangent lines to chain. However when you select rail 2 on sketch 2 at 3:27, tangent chain is still on and I found with that line/spline in that my equivalent to your sketch 2 (sketch 18) would 'tangent chain' select and mess up the loft. I wonder if calling it 'tangent chain' is not a little misleading in this respect. I wonder if it just means 'select lines that form a profile' and are closed out effectively.

If I turn off tangent chain however, I can loft between the same (sketch 20) profile you used and the point at the end of the original spline on sketch 16.  If is not a particularly smooth loft but it does work.

I would be really interested to hear your thoughts. I am really don't mean to lecture I am just trying to come to an understanding of how well I know Fusion 360. I have only just started posting here so I hope I am not offending anybody.

[Anonymous]

could it be that when i lofted, it didn't want to make a flat surface where the big face was because it was still trying to spin it on the guide rail, but could because it wouldn't be a curved shape? So the solution to my problem would have been mirroring over the smallest base and lofting then?

PS: sorry for run on sentence, had to get my idea down on text 🙂

[etfrench]

The main reason for starting with a fresh new file is to organize it according to Rule #1.  It will make it a lot easier for you as you get further along in the design.  The Patch workflow may give you a better shape for the blade, so you may want to experiment with that as well as the loft.

[beresfordromeo]

Hi etfrench

I am not sure what your mean here but my hunch is that you are partially right. I don't really understand how the loft rails but hope to one day.

The reason you got that specific error message I think is because there was one tiny stray line in Sketch 20. It was a line which intersected the spline on the sketch used in your video for Profile 1 I don't why it makes the loft produce that error but if include the missing bit circled the loft works. I think you must have included the missing bit in your first loft but not in the second that you recorded for the screencast. 

I only found this when repairing Sketch 20.