Using Fusion360 to produce drawings for 3D printing

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metalmuncher
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Using Fusion360 to produce drawings for 3D printing

Post by metalmuncher » Thu Aug 20, 2020 6:40 pm

I saw that someone in the sketchup & 3D printing thread asked if a similar one could be done for Fusion 360.

This is in two parts, a video and a writeup. The video is just a screen recording with no audio, the explanation is in text form below. I havent gone into complete detail on what every little tool does and how it works, there are better tutorials than this for a complete beginner, but I hope it shows the general workflow.

As with many things, there are 12 ways to skin this cat, this is one way, showing off a few interesting features of Fusion. You may notice there are some similarities to the Sketchup way of doing things.

The video is under 3 mins long, remember you can slow down the playback using the gear menu. I had to sit on my left hand to stop myself using keyboard shortcuts, so if anyone sees anything magically happen without a mouse click let me know so I can explain what I did.



When making scale models, I like to set up a user parameter with the scale factor. This is the first thing you see me do:
1.jpg
"Name" is what you use to recall the parameter. I want to work at 16mm/1ft, so that is what I put in the expression field. Fusion understands quite a few units, and you can mix and match metric and imperial. Since a scale factor is a length divided by a length, it is unitless.

NOTE: If you don't have the parameters "Fx" button visible, you can find it in the modify drop down menu:
params.PNG
Next, I draw a square. I think the video is relatively self explanatory. The first step is to create a new sketch, and click on the yellow xy plane I want to draw on. I then use the rectangle tool to sketch the box, and use the dimension tool to firmly define the size as 45x45 real-world mm.
2.jpg
Now I use the offset tool twice to create the inset lines. You see me type 3"*sm32scale. You can do mathematics within a lot of the numeric inputs, so this takes 3 inches and multiplies it by the 16mm/ft scale factor defined earlier, resulting in a scale size of the offset of 4mm.
3.jpg
Now I start drawing the lines that create the separate panes. I first draw the required lines, not bothering to get them lined up or centred, only letting Fusion snap them perpendicular to the other lines already there. I then use the collinear constraint to force them inline where they should be.
4.jpg
Now using the equal constraint to make them all the same length. You can see in the video how this makes it so dragging the lines affects the thickness of bit between the panes. I finally constrain this last degree of freedom by dimensioning this size. All the lines turn black showing everything in the sketch is constrained.
5.jpg
Now we turn the sketch into a 3D body. This works similarly to Sketchup. You use the push/pull tool to create a 3D object, extruding the bits of the sketch you want to a certain height. I then do it again for the outer frame, but extruding by a larger distance this time.
6.jpg
You may find after the first extrusion Fusion will hide the sketch, to bring it back use the eye icon in the project browser:
sketch.PNG
At the end of the video, you see me use one of the most powerful features of Fusion. You can go back and change parameters, like a dimension as in the video, and the 3d model updates with the change. This means for example, we could make a different size window by just changing the first 45mm dimensions we put down at the start, and the model would update accordingly.

If anyone has any questions about a specific part I would by happy to try and help.
Last edited by metalmuncher on Sun Aug 23, 2020 10:14 am, edited 2 times in total.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by ge_rik » Fri Aug 21, 2020 8:13 am

That looks interesting and quite logical. My burning question - is it idiot-proof? Will I be just as likely to produce an unprintable shape with Fusion as I seem to be able to achieve in SketchUp?

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Fri Aug 21, 2020 10:20 am

metalmuncher wrote:
Thu Aug 20, 2020 6:40 pm
if anyone sees anything magically happen .....

If anyone has any questions about a specific part I would by happy to try and help.
Richard,
You know me and how long it takes for things to sink in! I've downloaded and deleted Fusion 360 several times in the past because I couldn't get my head around it, much the same as with Blender. Your video explanation of that helped tremendously, so when I saw this one one, I thought, "Aah..."
However I'm afraid I've fallen at the first hurdle! It's probably a version difference, but my F360 (v2.0.8809) doesn't have the Fx button and I've spent best part of half an hour searching for it, or a lookalike. Any suggestions, please?
Screenshot 2020-08-21 10.16.07.jpg

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Fri Aug 21, 2020 3:41 pm

Richard,
Ignore my last post, I've found the parameters input, it's a drop down item under 'Modify' now, not a separate fx button.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by metalmuncher » Fri Aug 21, 2020 6:09 pm

ge_rik wrote:
Fri Aug 21, 2020 8:13 am
That looks interesting and quite logical. My burning question - is it idiot-proof? Will I be just as likely to produce an unprintable shape with Fusion as I seem to be able to achieve in SketchUp?

Rik
I would say Fusion's modeling system is far more robust than Sketchup's.

Sketchup's tools for the most part work on the basis of triangle models. A square face is really just two triangles for example, and that's why you get faceted arcs and circles in sketchup, its an approximation using triangles. Sketchup has no real concept of the mathematical definition of a circle or arc. You also have issues with backfaces and manifold geometry in sketchup that can cause issues with 3D printing.

Fusion's CAD model system is more mathematical than sketchup, it understands circles are fundamentally curved and not made from straight lines, and has robust tools that allow you to combine simple shapes into a bigger more complex one. You see at 2:03 in the video at the bottom of the dialog it says Operation: Join. This means the second, deeper extrusion will be joined to the first one, Fusion will take care of the cleanup work, making sure there isn't some invisible boundary face between the two different extrusions where they meet. You can also change that to other operations, such as cut. So, for example I could extrude the entire window to some thickness, then do another extrusion that cuts away the first to create the holes for the panes.

I don't think there is a concept of back faces in Fusion's CAD workspace like there is in sketchup, so that can't be an issue. Fusion will generally throw errors if the geometry you ask it to make cannot be created while keeping a solid 3D shape, for example if there is not enough space to create a fillet.

Fusion does actually have a system (mesh workspace) that can work with triangles directly like sketchup does, I haven't found it very useful apart from editing downloaded STL files. STL files are made of triangles, so when when it comes to export, the curved surfaces in Fusion do get turned to triangle representation as that's what the slicer understands, but that is the last step before printing, so you don't have to worry about it when drawing your model.
philipy wrote:
Fri Aug 21, 2020 3:41 pm
Richard,
Ignore my last post, I've found the parameters input, it's a drop down item under 'Modify' now, not a separate fx button.
Whoops, I thought my toolbar was reset to the default layout. You can customise what buttons are in the toolbar by clicking the dropdown in the pane, then the 3 dots next to the item you want to add to the main toolbar and ticking/unticking pin to toolbar. I'll add a note to the first post so people know how to get to it.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Fri Aug 21, 2020 6:23 pm

Thanks Richard, that works well :D

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Sat Aug 22, 2020 7:35 am

Sorry, me again.

I can't get the Offset to accept the full expression in your example. ( 3"*sm32scale ). When I do it, the 3 by itself is fine and draws a square 3mm outside the original. 3" also works and draws a square 3 inches ( 76.2mm) outside the original.
However, as soon as I add the * the expression all goes red and nothing else works. I must be doing something wrong I guess, but can't for the life of me see what?
Screenshot 2020-08-22 07.30.08.jpg

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Re: Using Fusion360 to produce drawings for 3D printing

Post by metalmuncher » Sat Aug 22, 2020 9:00 am

philipy wrote:
Sat Aug 22, 2020 7:35 am
Sorry, me again.

I can't get the Offset to accept the full expression in your example. ( 3"*sm32scale ). When I do it, the 3 by itself is fine and draws a square 3mm outside the original. 3" also works and draws a square 3 inches ( 76.2mm) outside the original.
However, as soon as I add the * the expression all goes red and nothing else works. I must be doing something wrong I guess, but can't for the life of me see what?
Screenshot 2020-08-22 07.30.08.jpg
It sounds like there is something wrong with the parameter setup? Did you make sure to set it to No Units? By default the parameters are set to length, so when you try doing inches * mm it gives an area, which doesn't make sense for specifying an offset length. Can you show your parameter dialog?

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Sat Aug 22, 2020 9:18 am

metalmuncher wrote:
Sat Aug 22, 2020 9:00 am

It sounds like there is something wrong with the parameter setup? Did you make sure to set it to No Units? By default the parameters are set to length, so when you try doing inches * mm it gives an area, which doesn't make sense for specifying an offset length. Can you show your parameter dialog?
I think that was it. Not sure what happened because the first time I did it, I didn't change to 'no unit's and it didn't work, so I went back and checked and changed it to no units, but it still didn't work. I've just redone it from scratch and it does now seem to be working Ok, thanks.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Sun Aug 23, 2020 8:36 am

Richard, a couple of Magic Moments for you. :D

At 1:52 in your video, the Select arrow magically becomes an Orbit tool. I did eventually spot that the LH tool at the bottom of the screen had gone a bluish colour but it took me quite a while to notice. I presume you used some sort of shortcut, off screen?

Now, I've finally got to the extrude section. I can select the inner frame and cross frame and pull them up the correct distance, exactly the same as your video. I get a two colour hollow effect, as in the video, but then in the video it suddenly all goes green, before you do the second extrusion. I can't find how you make that colour change action. Everything I do makes the extrusion go solid and deletes the the outer frame lines before I can extrude them.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by metalmuncher » Sun Aug 23, 2020 10:11 am

philipy wrote:
Sun Aug 23, 2020 8:36 am
At 1:52 in your video, the Select arrow magically becomes an Orbit tool. I did eventually spot that the LH tool at the bottom of the screen had gone a bluish colour but it took me quite a while to notice. I presume you used some sort of shortcut, off screen?
Shift + middle mouse button allows you to orbit at any time. Just MMB is pan as well. Very useful shortcuts, as it means you can move the view without it interfering with the use of other tools.

I think I just hit enter after typing 3 for the first extrusion, it's the same as hitting OK on the extrude dialog to the right.
philipy wrote:
Sun Aug 23, 2020 8:36 am
Everything I do makes the extrusion go solid and deletes the the outer frame lines before I can extrude them.
It sounds like it is hiding the sketch after the first extrude, you can hide/unhide the sketch using the eye icon in the project browser:
sketch.PNG

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Re: Using Fusion360 to produce drawings for 3D printing

Post by philipy » Mon Aug 24, 2020 7:17 am

Well I really hate to admit defeat, but I've come to the conclusion that I'm the old dog that can't be taught new tricks.
I've spent a total of over 8 hours, reading, watching, looking at help files and drawing ( I think I've started fresh drawings 7 times) and I still can't get this very simple project to complete.

Thanks for your attempts to educate me Richard, I do appreciate them, but Fusion 360 ain't for me. For all of it's faults, SketchUp is so much easier and more intuitive and I've never found something I can't make it do even if I have to bodge it!.

FWIW, when I was still working I went on an official Autocad course and came out of that unable to do more than very basic operations on Autocad LT.

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Re: Using Fusion360 to produce drawings for 3D printing

Post by Paul_in_Ricky » Tue Sep 01, 2020 9:50 am

Firstly, thanks for a great thread. It's further inspiration to make the effort to learn more about Fusion.
I probably wouldn't have thought of using the parameters function at all, but I can see that it could be really helpful bringing measurements into a drawing.

I've used Tinkercad a fair bit. Whilst it's the easiest to get started with, once you hit it's many limitations you have spend a lot of effort finding workrounds to get the result you need. Even then bits end up looking rather rather clunky.
Sketchup has never been a product I've liked. It's just too easy to make mistakes and impossible things, but awkward to manipulate and place items.

The problem with Fusion is it's power and huge range of options. Trying to find the learning resources for our particular requirements isn't easy. Tutorials often expect different usage, but even solo users have to use the same versioning and cloud based collaboration tools. I hope it will be worth the time invested in learning it thoroughly.

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