Fusion 360 - how can I draw panel lines for 3D printing?

[bootneck]

I am plodding on with learning Fusion 360 and, to be honest, I am pleasantly surprised how well it is going.  I do have a problem though, which all the tutorials I've watched don't seem to answer;  how can I draw very fine panel lines that will transfer over to STL and print?   I have no problems drawing the lines in Sketch Mode but that doesn't show as a line in the Bodies or STL.   If I use the Offset Tool, followed by an Extrude to make a Body, I find that I end up with a trench rather than a narrow panel line.

 

cheers,
Mike

[Graham Boak]

When you find out, pass the answer down to Airfix who appear to have the same problem.

[Alvaro Rodriguez]

9 hours ago, bootneck said:

I find that I end up with a trench rather than a narrow panel line

 

Well... may you be so kind to define "trench", please? 😅

 

Just saying because we do not know which one your model or scale is so it´s hard for us to know what you are refering to exactly.

 

Leaving apart the steps you follow for creating a panel line what matters here are the real dimensions -width and depth- and if those are printable actually. Note that a panel line that´s printable in a vertical face may not be printable in a horizontal one. These are common printing constrains and the usual suspect of such undesired result uses to be overexposure often. 

 

Others experiece may vary but I do not use to model panel lines under 0.2mm width as a general rule if I want my model to be printable by any end user and using any resin printer. If I´m doing a desing for myself and my printer I could go a tad narrower to 0.15mm or 0.1mm but that will depend on the face and depth.

 

Note the deeper a panel line -or a hole- is the more chances it will print partially or completely filled -because that depends on its width-. Or, in other words, if you want a rather depth panel line there is a minimun width for ensuring it is printable. Your experience, printer settings and printer performance will tell you exactly which ones such thresholds are for both minimun width and depth.

 

On a side note, I do my panel lines drawing then as beams in the sketch and not as lines. Then I just need to extrude for projecting them into the model surface. You could also create a new body and apply a cut. One of the good things of CAD is that there are many different approaches for the very same problem.

 

Regards!

Alvaro

[Tony Andrews]

I don't proclaim much expertise but here's a few options. None are very pretty and all have limitations.

 

1: Emboss. Only if the surface of the body is not too complicated (2D curves extruded are probably OK, 3D curvature probably not OK). Create a sketch and draw some long thin rectangles with the width you want. The positioning can be adjusted during the emboss process so the rectangles don't have to be aligned exactly right. Close the sketch and select EMBOSS. Pick the rectangles on the sketch and the face on the body then DEBOSS and enter the depth of the panel lines.

Big pluses of this approach are that the position of the lines can be easily adjusted, the lines wrap around the body, and it is easy to apply a fillet if desired. Downside is that you need a relatively simple surface or it won't work.

 

2. Cut through a surface layer. Break the body into two pieces comprising its outer surface and the main bulk. One way to do this is to use SHELL to create the "skin" with the depth desired for the panel lines, then reproduce the original body and use offset face to move it inwards to fit inside the "skin". Next create a new sketch on a suitable plane and draw long thin rectangles to match the panel lines you want. Switch on only the skin body and extrude from the sketch to cut through the body.

As the extrude only goes in one direction you cannot wrap around a body in one go so may need to do several sketches in different orientations to create a decent approximation, e.g. side, top, 45 degrees top-side, 45 degrees bottom-side.

 

3. Project to surface. Create a suitable plane, preferably in front of the body. Create a sketch on this plane and draw lines to match the panel lines. Close the sketch and create a new sketch (sketch plane doesn't really matter). use CREATE -> PROJECT/INCLUDE -> PROJECT TO SURFACE. Pick the face on the body, the lines on the sketch then ALONG VECTOR and choose a suitable axis (most likely normal to the sketch plane). This creates lines along the surface of the body which should match your panel lines. Next CONSTRUCT -> PLANE ALONG PATH and pick one of the lines on the surface of the body. Now create a sketch on this plane and draw the cross-section of your panel line, e.g. a rectangle with a rounded end. Now SWEEP this sketch along the line.

This does a good job at fitting around quite complex shapes. The ends of the sweep may have glitches due to the 3D orientation of the path. This can be resolved by an extra cut at the end of the path. As a trick you could also add material to the body first so the swept path can be made longer, then project the lines, sweep the cut and finally cut off the extra material.

 

Any better suggestions would be welcome

 

HTH

 

Tony Andrews

[wellsprop]

Projecting onto a surface is one of the methods I use that works very effectively (albeit in CATIA). 

 

I use a thickness and depth of 0.3mm for panel lines, which works out quite nicely. 

[bootneck]

Hello Alvaro, Tony and Ben,

 

thanks for your responses, there are some interesting pointers there and I shall have a look at using them tomorrow.  Althogh I mentioned panel lines, I just used that as a most common way that people might understand about thin grooves.  I tend to work to 1:144 scale and, although that tends to be small, I am working on a very large ship model.  I have lots of areas that require marked lines, similar to panel lines, such as plating and planking.  One such area, and the reason for my request, is the planking of the catapult launch area of an aircraft carrier. 

Immediately in front of the jet blast shields is a cutout area that is filled with flame-resistent planking and it is the line between each plank that I mean when I refer to panel lines.  This is a view of the catapult launch area that I am talking about:

 

As can be seen above, there is a single line, on the right hand side of the jet blast shields, and this is the edge of a series of planks that go from the lower side JBD across to the upper JBD.  That line is too thick and I am trying to find a method of making it narrower because I have about a dozen or so planks to represent there.  I am not at my workbench at the moment so I can't give any specific measurements but, as I say, the lines would really just be that.  If I was using my cutting machine then I would just Score the lines into the deck, or use a scribing tool; however,  I am trying to learn how to use Fusion 360 and this would be one aspect that will help me to understand and use more of the functions than I am currently used to.

 

Any information that I can get to resolve this would also be useful for when I start building my aircaft to go on this deck.

 

Thanks again for all your input and I would be very grateful if I can get any more helpful advice.

 

cheers.

 

Mike

 

 

[Tony Andrews]

If you just want to put slots in the flat surface then the easiest way is to put a sketch on that surface and then extrude into the surface, which looks like what has already been done for the recesses for the blast deflectors.

 

If you have simple straight lines then drawing rectangles is probably easiest with the width of the rectangles set to the groove width, e.g. 0.2-0.3mm. Any less will almost certainly not show up in the print - 0.2mm is only about 4 pixels .

 

If the pattern is more complex then it is probably best to draw the shape as a line then offset +/- by half the groove width and join up the ends of the lines to make an extrudable shape.

 

The depth of the groove is controlled by the extrude. The profile of the groove can be tweaked by applying an angle in the extrude and/or adding fillets or chamfers to the outside edges or bottom corners of the groove.

 

If there is a regular spacing then you can use the rectangular pattern to reproduce one groove either by copying lines in the sketch or features in the 3D body. Again, you have probably already done this for the structure on the back of the blast deflectors.

 

HTH

Tony Andrews

[bootneck]

thanks again Tony, and to all who have contributed.  I followed some of the advice given last night and I think I've cracked it.

 

 

 

 

 

 

I used the rectangle method, with a width of 0.03mm and then did a negative Extrude to 0.02mm.  The lines look good to me.

 

Thanks for the help and advice.  If you think of any other tips and tricks then please add them in this 3D Printing Basics thread, as I'm sure that not only I would benefit from such help.

 

cheers,

Mike