Importing a 3 view diagram to help create a model

[kdpinchie]

Hi all

I am trying to use Fusion 360 to help with designing scale model aircraft for 3d printing.

I thought I would be able to import a 3view diagram of the aircraft onto each of he X, Y and Z planes and go from there, however I cant seem to get things to happen like I hoped.

The aircraft I am trying to model is the CAC Boomerang, which I have found a reasonable set of drawings for, which include various cross sections which I am hoping will help with making the modelling more accurate.

Thanks in advance and apologies if this is a rehash of earlier questions / threads

[TheCADWhisperer · Accepted solution]

You can use image editing software, like MS Paint, to trim up your sheet into different images and then insert into Fusion Canvases.

I think this process is covered in the Tutorials.

[davebYYPCU · Accepted solution]

How is it that you are stuck?

i have done this a few times....

Using the same document, insert as canvass. Insert > Canvass three origin planes - three times.

Then Calibrate them to the scale you want.

I suggest you use the wingspan, and fuse length.  

By that I mean you can Calibrate the canvass front view and then top view, with the wingspan (to reduce errors with a longer measurement.)

make a sketch on the top view and draw a datum line for fuse length, measuring it.

Then Calibrate the side view fuse to that length.

Bit to go yet - don't know your level of expertise.  In the end you want all to be aligned to and be squared to the origin.

Edit canvass - (front first) move the centre of the spinner to the origin. Rotate canvass to be square, to the origin.

Edit the sketch with side view datum in it, so that it is attached to the origin.

Edit canvass - (side view) move profile of spinner to origin. Rotate .....

Edit canvass -  (top view) move front of the spinner to origin. Rotate.... etc.

Should get you unstuck.

Away from my Fusion machine for another week or so.

Browny.

[kdpinchie]

Thanks TheCADWhisperer and davebYYPCU

This was the piece of the puzzle that I was missing.  Last time I did any thing like this was a few years ago in SW2007 so I am having to learn a whole new way of doing things and the terminology for making it so

Cheers

[kvlasblomQYQWD]

I've managed to follow that description and now have all three views (sketches) scaled and positioned with the tip of the spinner on 0,0,0. What would you recommend someone do next to create a 3-D shell from this?

[TheCADWhisperer]

Have you gone through the Tutorials?

Can you Attach example of a previous project that you have completed?

It appears to me that you have already done too much work with a lot of repeated geometry.

I would expect to see about a year's worth of previously successfully completed projects of increasing complexity leading up to this project.

[kvlasblomQYQWD]

Thanks for your reply. I have followed tutorials and worked on two projects. One was measuring all the components of a model engine and drawing and assembling them on Fusion, the other (which incorporates the engine) is a model aircraft but by piecing together individual components that I had already drawn in another application in 2D (DraftSight), uploading the 2D sketches and then extruding them. I now wanted to see if I could learn to avoid using another application in combination with Fusion, and only use Fusion. My hobby is building and flying scale model aircraft, so I will always be starting with a 3-view drawing, 3-view photos or both. I thought that if I could draw the basic outlines in 3D, I could then split that to create formers (cross-sections of the fuselage and or ribs in the wing) and the constructional detail from that.

- Completed drawing of the engine: https://a360.co/2Q1TM1y

-Saab Safir 1:4 (Work in progress) https://a360.co/2OnAciH

-The third page of my thread on a Dutch modeller's forum which shows some pictures of my work on the engine https://www.modelbouwforum.nl/threads/saab-91d-safir.249679/page-3

The 3-view I found to use as a learning project was actually an .svg file instead of an image, so I projected the lines from that to new sketches to put at the origin point. This project for a Piper Cherokee was just to play with, to learn the technique required to achieve what I described above. I learn quickly but need to be instructed the first time around 😉 

[TheCADWhisperer]

I saw unconstrained geometry in your sketches.

This should be mastered. 

Now it may be a bit more freeform for you airplane body, but if simple lines and arcs are not defined in prismatic geometry...

[kvlasblomQYQWD]

In which project? This one that I'm playing with I did not do the sketches for, I merely projected the lines and curves from the downloaded file to quickly see what I could do to make a 3D form from the 3-view.

[laughingcreek]

It sounds and looks like all those sketch entities are imported geometry.  creating 3d geometry from imported sketch curves is a dicey situation.  Works sometimes, many times does not.  It' not a solid work flow. 

It is always suggested that curves drawn natively in fusion be used to create solid features.  So that wold be the next step.  Identify the part of the plane makes since to create first,  think about the solid features that could be used to create it, and draw the sketches you need.   

early in the process you should start a new thread and post a question, along with your exported and attached .f3d model, to get help and pointers.

(ps, don't use those link for sharing.  The ones you posted above don't work.  even when they do work they it's a PITA for people trying to help you.  Much easier for everybody if you attach the actual .f3d file to the post)

[TheCADWhisperer]

---

@kvlasblomQYQWD wrote:

In which project? 

---

The engine.

I look at the history of completed project to try to gauge experience level of the user so that I know when level of help is needed.  How to sketch a line of known length, or can we start on overbuilding and then trimming a surface body...

[davebYYPCU]

In addition to the advise already given, an overview, 

I build all parts in place, with timeline history, won’t draw anything twice.

Build from outside > in.  I use Surface bodies then Thicken, for our work, Solid and Shell is less reliable. Wing and Tail TE’s to a sharp edge, for example.

Make your Fusion workings, fit for your desired output, which is?

to create drawings, create dxf for 2d Cutting, or 3d toolpaths,

should be what drives the designing.  Took me a long time to find the 3d workflows that suited me.  Fusion has some bugs but it’s doable.

I use a component for the large sections, with many bodies, progressing to sub component for each part to output.  

Example, Wing is component, sketch required geometry, end Ribs, then bodies for skin, spars, servo Rails, servo cable tubes, push rods, hinging, etc.  when done, ribs are extracted and made into subcomponents, last.  A workflow that suits me for Laser Cutting.

In your Cherokee example, you will see there is a few missing profile shadings, so already there are gaps in the geometry to fix, and

You have a component for each view sketch, I would keep those at the top level, with the canvasses, or referenced as if they are canvases.  Again for the Wing, only bring into that Component what you need for a half wing to be mirrored late.  You don’t need all those corrugated skin details, to make the flaps and ailerons.

I will check the other files, but a few clues for now.

Might help....

[davebYYPCU]

I have viewed the Saab, and see it's imported 2d for inside > out.

My experience is that this method does induce more errors.  You are reliant on the original drafting by measurement.

In Fusion making formers or ribs compliant to the outside dimensions works better for me.

Might help...

[kvlasblomQYQWD]

That's right. I drew in 2D, but during that project found that the plate that holds the retractable undercarriage needed to be tilted in 2 or 3 dimensions. The exact measurements of its edges became too complicated to imagine and draw in 2 dimensions so I decided to learn to use Fusion. That turned out to be addictive and then as I drew the parts in 2D (other software) I decided to add them into the 3D environment in Fusion. For future projects I thought I ought to learn to design the entire model in Fusion, from existing 3-views drawings or photographs as canvasses.

[kvlasblomQYQWD]

Thanks Dave. I understand I should throw this away and start with a clean file. 

And start a new thread for the project for help here. 

So would you say then that I should:

-Place three canvasses on the origin, all scaled and lined out properly,

-Draw my own sketches with proper constraints over the canvasses,

-Draw sketches as formers throughout the fuselage

-Add sketch points to aid the use of the loft tool to create a 3D exterior shape

...and then to use that to create the interior construction?

[kvlasblomQYQWD]

Here is my messy file attached.

[davebYYPCU]

Not start again, those sketches, aligned to Origin planes, will be real good start.

Happy to help, if you get stuck.

[chrisplyler]

There is nothing wrong with having those three SVG sketch imports instead of having three Canvas images. In fact, it's even better.

As an example of workflow, let's talk about the prop spinner.

Create a new Component. Rename it 'Spinner.' Since the spinner's point is on the origin, you won't need to make a Construction Plane there. Create an Offset Plane, select the To Object option, and choose a line or point at the rear of the spinner. Create a new Sketch on that Offset Plane. Project a point from the SVGs that gets you an appropriate center point. Project a point from the SVGs that represents the outer radius. It may be useful to Project>Intersect any of the SVG lines that pass through your sketch plane in order to get the desired point(s). Center a circle on the first point and radius it to the second point. That completes the rear of the spinner cone. Finish that sketch. Start a new sketch on the origin plane that is parallel to the first sketch. Just put a point on the origin that will represent the point of the spinner cone.

Now you've got two sketches within the Spinner component. One with a point and one with a circle. With the Spinner component still activated, Loft from the point to the circle to create the cone. Play with the Loft setting options to develop the shape to your liking. You can do this as a solid and then Shell it from the back, or you can do it as a surface and then Thicken it afterwards.

Of course, you could have done it with a single sketch, projecting in half the spinner's section shape and then Revolving it. But that method isn't going to be adequate for MOST of the craft's components, so I thought to go ahead and get you started lofting things. Many of your shapes will require more than just a front and back sketch, needing one or more 'intermediary' sketch profiles in between those two. But for the spinner, probably not.

Now you will probably need planes and sketch either side of the spinner in order to Extrude/Cut out the sides to fit around the prop blades. And you might need to get a screw hole close to the rear to pattern around. I don't know how detailed you're wanting to get.

When you're done with the spinner, create a New Component and rename it 'Spinner Rear Plate'. You might be able to do this with only a single sketch of the section and Revolve it around inside the spinner. Then an additional sketch to Extrude holes through the backing plate as required. You may be able to get holes through the perimeter flange that are dependent on the spinner's rear holes as required.

Anyway, keep making New Components and modeling the contents of each one as required. Each component should represent/contain a single part. You can nest components together into an assembly, for example putting all those related spinner parts into a single assembly. This will help keep your Browser manageable.

Quick review: Put those SVGs under the topmost Browser hierarchy and just use them as guides., and then make components/assemblies that each have their own simple sketches to define the bodies therein, BASED off of those guides.