topic Re: Problem with Loft in Fusion Support Forum

Problem with Loft

Anonymous — Thu, 16 Apr 2020 09:34:11 GMT

Hi all,

I'm new in the forum and I started to work with Fusion only few weeks ago.

I have to generate a solid starting from two skatches in two parallel planes (joining the two profiles).

I tried first to generate a Loft but nothing reasonable is coming out and surfaces are intersecting each other in a "stupid way".

Please find attached the file where the two skacthes are and a picture of the solid I have to design...just to give you an idea.

I'm getting mad for probably something some of you will find simple.

Please help if you can.

Thanks a lot in advance, stay safe,

Andrea

Re: Problem with Loft

davebYYPCU — Thu, 16 Apr 2020 09:56:40 GMT

Imported sketches with hundreds of small lines or points,

Redraw it in Fusion. Most lower rebates are fine, just the top curves throwing the spanner.

Origin, symmetry, fully constrained sketches will make life easier too.

Might help....

Re: Problem with Loft

Marco.Takx — Thu, 16 Apr 2020 09:53:13 GMT

Hi @Anonymous,

The problem of your loft is that it tries to connect all points.

Try to make a cleaner sketch.

I've uploaded a model to show you.

I didn't use nice sketching. This is only for reference to the loft.

Have a look at it and give it a try.

If my post answers your question Please use Accept as Solution & Kudos This helps everyone find answers more quickly!

Re: Problem with Loft

Anonymous — Thu, 16 Apr 2020 10:00:23 GMT

Oh guys....

you were quick!

Thanks so much.

Marco I'll check your file (already had a look :)) and see what you did as example.

Thanks again and I'm sure I'll need you help again in the next weeks/months.

Have a safe day,

Andrea

Re: Problem with Loft

MoshiurRashid — Thu, 16 Apr 2020 10:10:10 GMT

Hi @Anonymous

As I can see, one of the sketch is created by so many vertex. However, I made them construction and redrawn the sketch on it. Then, I extruded the two bodies to opposite sides so that you get clean faces.

Now, all you need to do is to create some guide curves as your requirements. (I've created 2, watch them)

Then you can loft it with guide rails.

Re: Problem with Loft

davebYYPCU — Thu, 16 Apr 2020 10:48:37 GMT

Using OP sketches for the extrudes makes no difference, still making Loft use all the points. Only 2 rails is not enough.

Re: Problem with Loft

MoshiurRashid — Thu, 16 Apr 2020 11:39:36 GMT

@davebYYPCU

1. I did it for the upper sketch as an example and I let the user to do the below sketch.

2. I didn't say 2 rail is enough. More sketch is needed. I suggested the user to place rails as his requirements.

Re: Problem with Loft

TrippyLighting — Thu, 16 Apr 2020 12:17:34 GMT

My screencast shows a few techniques about how to re-sketch this with the tools in FUiosn 360.

1. Move the imported geometry so it is symmetric to the sketch origin. That will allow you to only sketch half of it.
Then I use the sketch tools to sketch half of a profile. You'll notice a few things
1. I don't put any fillets in the sketch! As a general rule ( with some exceptions) ff a fillet can be created using a modeling feature then it should not be in the sketch.
2. I dimension everything but the splines. I am too lazy to fillet the splines, but you probably should 😉
Once done with each half sketch I create a loft.
Then I apply the fillets.
Then I mirror. Don't mirror half sketches. Mirroring 3D geometry is better.

Hopefully this screencast posts. The cretins who "maintain" the forum software now have removed the HTML tag, which was the one way to ensure 100% success rate when embedding screencasts.

Re: Problem with Loft

MoshiurRashid — Thu, 16 Apr 2020 12:46:15 GMT

@TrippyLighting

Screencast didn't appear. Please post the link also.

Re: Problem with Loft

TrippyLighting — Thu, 16 Apr 2020 18:34:10 GMT

Here is the link to the screencast.

I've created over 800 screencasts and 2/3 of those I posted by using the HTML tag available in the toolbar right above the text editing field. This has worked without a single failure hundreds of times in succession. Let's hope they get that fixed soon!