Help please, drawing compound curves

[mthuff]

From the attached screenshot, you can see both ends of the ammunition-feed channels from a wartime FN5 turret, which I'm preparing to model. My difficulty is how to "twist" and simultaneously "curve" the constant cross-section to join the two ends of the channel. If someone could suggest a tutorial or other link, or indeed lay out a strategy for drawing this, I'd be most grateful, having expended many thankless hours to no avail.

[JDMather]

Is this an AutoCAD question, or is it really a Fusion 360 question?

In either case Loft.

[mthuff]

Hi, It's really a Fusion 360 question - I'm new to the forum and don't really use boards much. Apologies if it's in the wrong place. Are you able to punt it to the correct forum?

[BeKirra]

As JDMather said, "loft" is the command you may use. Another command you may want to try is "sweep".

Have you tried it out?

Give a simple practice for "sweep", start a new part file. On a sketch create a profile, then on other sketch create a curve path.

Now you may be able to create a sweep feature. You may also click the "?" button for help detail in the left lower corner in sweep dialog.

HTH

[davebYYPCU]

I agree that Loft command will do it.

Use face of A, and the face of B for profiles.

try pulling with weight.

In the dialogue box, click next to Free, and use direction to adjust the shape of your new part, each end will be adjustable.

if not happy with that, you will need the addition of rails.

Another way may work with Sweep with path and guide rail, 

either way, you need 3d splines for your Rails, or Paths.

Might help...

[davebYYPCU]

I will eat my words, the loft worked as stated, Weight of 0.7 was used both ends

If you realign the mapping points, 

but simulating as a block was okay, but simulating the channel, was a nightmare I declined to edit, 

So, Sweep with Path and Guide Rail is the way to go, (attaching the file)

I realise that to make the rails was where you were asking for advice, 

I have created two 2d sketches, and create the side and front view paths for the back face of the channel end points. (Could use any face)

Used Intersection > Curve to create the 3d paths.

Selected the channel profile and the two 3 d paths, in the Sweep command.  (Change for type in the dialogue box)

Use light bulbs and the step by step history marker to see what I did, but could make a screen cast if still stuck.

Might help...

[mthuff]

I'm sorry but. I've been unable to follow this, particularly the intersection curve part. I've looked at the file you sent, and can see how the planes are arranged, but not how the 3d curved paths are generated to use as guide-rails for the sweep.

I am most grateful to you for taking the time to help me get past this.

[SaeedHamza]

Hi,

Here is a quick screencast that shows that modeling this in an empty space is different from modeling it attached to both sides

And this can be solved using the loft in the Patch environment

Might help

Regards

Saeed

[davebYYPCU]

I hope this will be a clear explanation, I have presumed you know your way around Fusion, and concentrated on the Sweep with 3d rails,

If not let me know...

(Deleting the rails in the vid required a new Sweep Feature  - my bad.) 

[mthuff]

Thank-you ALL for taking the time and trouble to help me with this. I think I've probably got enough to work through this now, and will post a picture of the developed drawing when I look at it again later and done the feeds. I'm hoping to make several 1:4.5 scale model Frazer-Nash FN5 turrets in wood and aluminium, and have been "stuck" on these ammunition feeds for a good while now! I've only been using F'360 for about 6 months now, so to find this level of community support for dealing with my first enquiry is tremendous. Many thanks again.

[mthuff]

I've had a really good go at this this morning, but can't get the rails to draw, I fear the problem lies in confusion at to which planes to use, and why they're offset, to create the initial splines from which the 3d curves are developed. Would it be possible to upload a drawing for revision, or would you mind trying an explanation limited to the above? (I'm confident that once I've cracked that bit, I can create the bodies.)

Is it possible to upload a drawing here so someone can edit it by adding these double-curved chutes, then I can download the amended version to revise other areas:?

Thanks again to all who have tried to help

[laughingcreek]

Yes please! Uploading a sample of your issue is usually preferred.  Go to file-export and export as an archive file to your hard-drive, then upload it here.

[mthuff]

Neither .iges nor .sat file extentions seem to be uploadable from the export menu, so I'm unsure what I need to do to upload it. In the latter case I'm getting:

• "The attachment's FN5 Turret v98ducts for messing with v54.sat content type (text/plain) does not match its file extension and has been removed."

Sorry to be so clueless with this stuff.

[laughingcreek]

Export as a fusion archive file (extension .f3d), make sure the "save to my computer" box is checked.

[TrippyLighting]

Files/designs are needed in native Fusion 360 format .r3d or .f3z.

If your design is self contained .f3d is resented as a choice in the export dialogue.

For designs containing linked components/assemblies you should share a public link to your design.

[davebYYPCU]

I am away from Fusion till Sunday, and not used the new. Web Browser stuff yet, but, I know A360 does not show anything but bodies,

In my file those 2d offset sketches are on my origin planes.  I also made a plate to simulate that upright, to try to copy the information in your first photo.

My Origin is where the bottom left corner of the plate is positioned.  You can make the offset planes anywhere, the function still works.

Since I did that example, I realised that, making the first Demo Surface, is quicker and easier to do.

In the video where I say this twisted back piece doesn't exist but is for demo purposes,

(should have been my ah ha moment, in stead just a Seniors moment,  a wonder nobody jumped on to it)

I would now recommend that you make that surface, and disregard the constructed method from the video, 

When you have that surface made, Using Patch > Loft, with about 0.7 Direction weight both ends, 

Create 3d sketch, Use Project > Incude 3d Geometry, select both edge rails from the surface.  

Hide the surface body, you have 2 purple rails.

You can now Sweep the channel profile with them, 

So much simpler, and quicker.  Will see if I can attach the final version for you.

[mthuff]

This should resolve to a downloadable copy of the file, if someone can add the missing parts of the ammunition ducts either side, I'd be very happy! In the meantime I'll try and figure out how to achieve it myself, in order to know what to do next time the issue arises. It is likely a large file.

http://a360.co/2vWPCyh

Cheers,

[mthuff]

Thanks dave, I can't tell you how much I appreciate all the help, from all of you, on the first thing that's really given me trouble since I took up Fusion 360 a few months ago. Have a good weekend.

[davebYYPCU]

Best I can find out, that the Browser stuff is still not compatible with IPad, so see ya in couple of days.

[TrippyLighting]

The first thing I look at when helping other users with their designs is if there are any sketches in the top level sketch folder and then what these sketches are for.

It seems you should definitely review Fusion 360's R.U.L.E #1. It will make such an involved project much easier to deal with. It's a very nice design and considering the length of the timeline already and detailed design and I am surprised that you have persevered through it using a less than ideal workflow!

Secondly all, the bodies the top level bodies folder should actually be components but it might be too late to do that!

Also I performed a "Modify->Compute all" and there are 37 warnings (yellow and/or red icons in the timeline). You should consider fixing the before your design becomes unresponsive.

Lofting this with a solid loft will be a challenge even with plenty of guide rails.

Lofting this in the patch environment might work but will need many guide rails.

In general I am assuming that the two profiles were supposed to have the same cross section, but they don't exactly match.

Anyway, I did what you see in the screenshot below with a sweep with path and guide rails and pointed out where the profiles don't match.

You really need to get a better understanding of what the difference between an component and a body is in Fusion 360 and as already stated above follow Fusion 360's R.U.L.E #1 as stated above.