Jump to content

How to do canopy frames and panel lines in Fusion 360?


zebra

Recommended Posts

Title says it all really. I'm giving Fusion 360 a go, would like to add some panel lines, canopy frames and I suppose some other surface features will come up as well, what's the best way to add them to a surface or a solid in F360?

 

cheers

Julian

Link to comment
Share on other sites

I'm using CATIA v5.

 

For panel lines, I create a thick skin (the skin thickness should be the same as the panel line depth) of the entire airframe, remove the bits that are not panels, before subtracting what is now a load of panel lines from the main body.

 

This ends up with the model with some cutaway bits as panel lines. 

  • Like 2
Link to comment
Share on other sites

12 hours ago, wellsprop said:

I'm using CATIA v5.

 

For panel lines, I create a thick skin (the skin thickness should be the same as the panel line depth) of the entire airframe, remove the bits that are not panels, before subtracting what is now a load of panel lines from the main body.

 

This ends up with the model with some cutaway bits as panel lines. 

Thanks, I'll give this a go. What depth do you use for panel lines? I'm guessing at about 0.2mm.

Link to comment
Share on other sites

12 hours ago, wellsprop said:

I'm using CATIA v5.

 

For panel lines, I create a thick skin (the skin thickness should be the same as the panel line depth) of the entire airframe, remove the bits that are not panels, before subtracting what is now a load of panel lines from the main body.

 

This ends up with the model with some cutaway bits as panel lines. 

 

Ben, have you considered projecting lines onto the surface, and using them as a thin feature with an extruded cut?  (Offset from the surface )

I'm sure that would save a lot of work

Link to comment
Share on other sites

1 hour ago, hendie said:

 

Ben, have you considered projecting lines onto the surface, and using them as a thin feature with an extruded cut?  (Offset from the surface )

I'm sure that would save a lot of work

Do you know how to do that in Fusion 360?

Link to comment
Share on other sites

9 hours ago, hendie said:

 

Ben, have you considered projecting lines onto the surface, and using them as a thin feature with an extruded cut?  (Offset from the surface )

I'm sure that would save a lot of work

 

Hi Hendie,

 

You're quite correct, this does also work and it can be quite a bit quicker. Annoyingly, CATIA gets very funny about projecting lines that touch (or go over) the edge of a surface and therefore refuses to get them. The other benefit of creating a thin walled shell is the panel line depth is always constant as, rather than extruding the panel lines in a direction, the panel line depth is determined by the wall thickness.

 

@zebra, I'll try and find some online tutorials... I learnt all of my CAD skills from youtube - there are some fantastic resources out there :)

 

  • Thanks 1
Link to comment
Share on other sites

I use Rhino 3d and it really is a very simple process to create a set of vector lines either in Rhino or in a vector editor like Illustrator, project the lines onto surfaces, solids or subdivision surfaces.  From there you can sweep a profile or create a pipe and then use the Boolean commands to subtract, intersect or split.

  • Like 2
Link to comment
Share on other sites

On 1/12/2022 at 4:43 AM, wellsprop said:

The other benefit of creating a thin walled shell is the panel line depth is always constant

 

as it is when you extrude the cut using "offset to surface" option. The downside is that it doesn't always work if the surface is very complex so sometimes I have to use several discrete operations to complete the process. 

My home laptop wasn't built for CAD so I have to be conscious of file size.  The Wapiti build was about the limits of what it could handle without frustrating me too much

  • Like 4
  • Thanks 1
Link to comment
Share on other sites

  • 1 month later...

I've not done panel lines per se, but when I wish to introduce a surface line I tend to slice the model where I want it, bevel the edges (0.3mm IIRC, but not certain) then rejoin afterwards.

 

The lines in the horseshoe magnets on these 1:8 BTH magnetos were achieved like that.

 

spacer.png

  • Like 2
  • Thanks 1
Link to comment
Share on other sites

I am also interested to find an answer to Julian's query; the problem being, as I've only ever used Fusion360, I don't understand these worded theories.  Can anyone help by pointing me/us to some practical and visual step-by-steps please?

 

Cheers,
Mike

Link to comment
Share on other sites

Mike if you are really interested i could perhaps run a tutorial over teams or something similar? 

 

Need to find a file sharing site to post images... still haven't recovered from photobuckets policy change :)

  • Thanks 2
Link to comment
Share on other sites

That would indeed be great.   I just wish there was somewhere local that I could have gone to do one-to-one training on this, as I find Fusion 360 to be a very good application for me.   If you could set up something, then I'm sure that others, in a similar situation, would also like to know how to do things correctly.

I think most of us here suffered from the Photobucket changes; now, I find Imgur to be a good, and free, photo hosting site that is simple to use for posting on here.

 

cheers,
Mike

  • Like 2
  • Thanks 1
Link to comment
Share on other sites

10 hours ago, albertross said:

Need to find a file sharing site to post images... still haven't recovered from photobuckets policy change :)

A slight diversion but... I use a free Wordpress blog account. You can set a dummy front page, then upload photos to it without actually displaying them on the blog. If you edit the pic you can copy a link that will take people to it directly.  Wordpress allow you 3Gb of storage.

  • Like 1
  • Thanks 1
Link to comment
Share on other sites

On 3/1/2022 at 10:24 AM, albertross said:

Mike if you are really interested i could perhaps run a tutorial over teams or something similar? 

 

Need to find a file sharing site to post images... still haven't recovered from photobuckets policy change :)

I'd love to join in too. Time zones are always a bit of a challenge from here, but if it works I'm in.

 

cheers

Julian

  • Like 1
Link to comment
Share on other sites

So here we go how to create a sweep in Fusion for generating panel line / split. I'll use a similar shape to the mag cover.

Firstly we create our base sketch. For simplicity I've made the base shape solid. We will re use this sketch later for the sweep.

2022-03-01 (1)

 

Notice the lines are all black, indicating the sketch is fully constrained. Also note the vertical constraint between the arc centre and the origin point which is the mid point of the bottom line.

Also what you should be aware of is that every dimension has a unique identifier. This information can be re-used later on.

For example the 20.00 dimension is d1 (NB)

2022-03-02 (2)

 Once we have completed our sketch I extruded the profile equally from the mid-plane.

2022-03-01 (2)

We now create a sketch on our  xz plane. You could of course select the face. This is important as the plane and our original sketch our related. 

2022-03-01 (3)

 With our plane selected we now create the profile we want to sweep. This will generate our panel line.

On the sketch you can see the 9.75 dimension has an fx in front of it. This because I am using an equation to generate this position.

I have referenced d1 to create our depth. This means if we change d1 to 21.00 the panel line sketch is related and will move with the modification and not fail.

2022-03-01 (4)

 

Below is the simple equation 

 

2022-03-02 (3)

 

Now that we have completed the sketch we need to create the sweep. 

 

TBC

 

  • Like 1
Link to comment
Share on other sites

So selecting sweep from the create pull down menu

2022-03-01 (5)

 

We first select the profile we wish to sweep. So obviously we choose our triangle to create an indentation. (I have not printed using this style of recess any opinions on the matter would be interesting)

Hopefully you can see that profile is highlighted blue in the sweep dialogue box, and that the actual profile now it is selected is also blue.

 

2022-03-01 (6)

 

 So now we have the profile selected it is time to choose a path to sweep around.

In this instance we are going to use sketch one To make this visible (if it isn't already) select the correct sketch in the sketch tree in your browser flyout and press the v key (keyboard short cut)

Select path in the sweep dialogue box and then select the profile. Depending on your settings you will probably need to change the operation setting to cut.

 

2022-03-01 (7)

 

When all this has been selected you should get the above representation of what is about to transpire.

This is all good, but I don't want to actually have a groove in the bottom face.

Therefore back to the Sweep dialogue box. Here we can de select the chain tick box (Below path)

We can now de-select the lower line giving us the following result.

 

2022-03-01 (8)

 

Neat huh, so now we are ready to rock and and roll and hit the magic ok button to accept the operation.

With a little luck should end up with this. (exaggerated a little for clarity).

 

2022-03-01 (9)

 

 

Hope some of the above is useful. Don't forget there are many workflows to achieve the same result. This is just my preferred method.

 

All the best 

 

David

 

 

  • Like 2
  • Thanks 3
  • Haha 1
Link to comment
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
×
×
  • Create New...