Loft point Problem

[Anonymous]

Hi All

I have a problem, I have tried to draw the points to the correct position but it does not work any way.

[Pillnoob]

I could be mistaken but it looks like it may not like the bottom highlighted in Red line. Attach your file and maybe myself or another member can help. You can also make the shape you want and use a "cut/mold" command.

[Anonymous]

@Anonymous

I think you have to many points (ones that are not connected and are white) on both sketches.

1. Start with closed sketches on both planes
2. Draw guide curves (in 3D) if you want
3. Loft the outside profile
4. Loft/cut the internal profile
5. This is how the loft dialog looks like when cutting the internal profile

It all starts with good sketches.

[PhilProcarioJr]

@Anonymous

"I think you have to many points (ones that are not connected and are white) on both sketches."

The white points are the guide lines that the loft feature creates to help you control the loft, they are not user created.

@Anonymous

If you do single extrusion with guides like @Anonymous shows it will work fine, if you share your file I can show you how to do it all in one step using a single loft shown in your problem pic lining up the guides.

[Anonymous]

@PhilProcarioJr In principle you're right, the white points are created by the loft tool, however, top right in the back profile, you can see there are 5 points that are created for no apparent reason.

[PhilProcarioJr]

@Anonymous

You misunderstood my post, I wasn't disagreeing with you, only trying to point out that there are a lot of times the generated guides in Fusion twist for no apparent reason (even when the sketch is right) and people new to the software should know how to solve that with the guides. In addition to your answer (which I agree with your solution) I was trying to show @Anonymous how to deal with the auto generated guides. Nothing more, thus why I gave you Kudos for your post.

[Anonymous]

@PhilProcarioJr thanks, just thought i missed something as you have good nuggets every now and then 

[PhilProcarioJr]

@Anonymous

As you can see in this video I have clean sketches and it does the same thing as in @Anonymous example.

The reason your solution worked so smoothly is because of the guides, and it is also the reason the auto generated guides did not get messed up.

Your example is definitely the best way to handle the problem (clean sketches with proper guides) but doesn't solve more complex lofts where even guides don't help, and you still need to fix auto generated guides. My intention was only to show them how to manipulate the auto guides to resolve issues where manual guides fail.

[Anonymous]

Thank You all, new clean Sketch helps....

[jeff_strater]

Hey @PhilProcarioJr, what is the trick to getting Fusion to produce the wrong point mapping?  I tried a simple case, and it seemed to work OK:

I'd love to pass this on to the loft team, because this seems to be a case where we could improve the default point mapping.

Jeff

[edit]  Never mind...  As soon as I posted this, I found the trick - just to have the indents not lined up geometrically:

[PhilProcarioJr]

@jeff_strater

Offset the notches more... I run into stuff like this everyday running Fusion. Granted adding your own guides cuts that number way down but simple shapes shouldn't have problems like this. You can clearly see in the file that the sketches are clean with no extra points along edges.

Screen cap of a new file with the problem...

[PhilProcarioJr]

@jeff_strater

Here is another case that fails without guides...

The worst part about this one is if you select the bottom first it at least trys to create the loft but the other way around it flat out fails.

 https://knowledge.autodesk.com/community/screencast/052613be-0445-4861-a374-84518b71bc9f

[PhilProcarioJr]

@jeff_strater

Here is one more in case the first two don't help....

[Anonymous]

@PhilProcarioJr in all fairness to Fusion, other cad would not even loft this and gives you an error as to self intersecting geometry.

[PhilProcarioJr]

@Anonymous

I knew you were going to say that, so before I posted the 3 examples I ran them through Solidworks, ZW3D and had a friend do them in Pro-E all were able to do them fine.

Here is the proof for Solidworks...created the exact same sketches and used the loft tool..no guides...

[Anonymous]

hahaha @PhilProcarioJr that's not the same sketch. As I have tried your sketch in Solidworks and it doesn't work.

Also, notice where you clicked to create that loft.

I take that back. After another try it does indeed work.

[PhilProcarioJr]

@Anonymous

That is the same sketch and that's the point Solidworks allows you to guide it through your selection.

Either way believe what you want..he asked for examples so they could improve the code..all I did was what he asked.

[Anonymous]