Looking for Fusion 360 tutorials specific to front panel making

[substitute]

I'm thinking about buying a hobby cnc machine for making my own front panels, but I figured before I pull the trigger I'd spend some time with the software to see how I get on with it. I've been messing with fusion 360, I get some of the basics , I can make shapes and holes and setup tool paths but I'm getting super confused by trying to add text.

-What is your workflow for front panel design? Do you do the entire thing in CAD or import a SVG from illustrator then do the 3D work?
-How do you do text? Do you use 2D pocket or engrave function? What bits do you use?
-Can you recommend any tutorial videos specific to front panel making?

Thanks

 

[totoxraymond]

Hi,

I don't think you need fusion 360 for front panels, it's mostly a 2d job.

I make my own front panels with a small cnc and my workflow is mostly open source and free and is as follow:

1_ Qcad for drawing the front panel but I might switch to Front Panel Designer in the near future. Any 2d CAD might work as long as you can export dxf. The trickiest part is to find a font compatible with cnc engraving (single line) qcad has a few.

2_ dxf2gcode. A nice software  which i use to generate the gcode from dxf file. It's quite complete but lacks a few options. If i need to mill a pocket, I like Cambam to generate that specific gcode (i don't use pockets much so i've used a demo this far)

3_ bcnc/grbl to actually control the cnc. It's a nice open source solution that even runs on raspberry pi, with all the options for probing, tool length...

Learning how to use a cnc is note easy but very satisfying in the end. It takes a few trial and errors and several bits breaking/flying around your workshop.

Wear safety goggles / earpads! Always!

Never leave you cnc alone, even for a few seconds.

Have fun!

Thomas

 

[substitute]

Thanks, I'll check out those suggestions. I'm definitely not married to 360, the appeal is, it's free, it's well supported, and if I get into 3d printing or other more advanced CAM I'd have a knowledge base to build on. The downsides of course are weeding through a ton of functionality that has nothing to do with my goals.

1_ Qcad for drawing the front panel but I might switch to Front Panel Designer in the near future. Any 2d CAD might work as long as you can export dxf. The trickiest part is to find a font compatible with cnc engraving (single line) qcad has a few.

What bit do you use for fine text?

I like Front Panel Design, it's a little quirky but ultimately quite easy to use. I did a quick rack panel layout with a few holes and some engraved text, exported as dxf and loaded into 360. When I extrude the sketch all the holes translate perfectly and setting up tool paths is easy (granted I'm not worrying about dialing in operating specs) but the text is all weird. Like only some parts of some letters survived the extrusion process. 

Again, really interested in checking out some of that 2D stuff, I kinda just want to get this going and don't really care about learning a whole new software platform.

 

[substitute]

2_ dxf2gcode. A nice software  which i use to generate the gcode from dxf file. It's quite complete but lacks a few options. If i need to mill a pocket, I like Cambam to generate that specific gcode (i don't use pockets much so i've used a demo this far)

crap, checked out dfx2gcode, all that python stuff is totally beyond me, I don't know what any of the words in the installation instructions mean.

I've made some progress, adding text with in 360 seems to be working out now. It's really importing dxf or svg files that seems wack-a-doo.

 

[totoxraymond]

What do you mean about Python? I've used dxf2gcode for quite a while and never had to deal with python (or any scripting language).

For engraving, I use a "pointe javelot" (don't know how to translate in english) 25°
the same as the one linked below, but in 25° instead of 30° (it seems they don' t sell the 25° anymore)

https://www.cncfraises.fr/pointes-javelots-1-dent-carbure-evomax/323-pointe-javelot-1-dent-30-degres-evomax-carbure-pointe-0-1-mm-queue-3-175mm.html

I'm not suprised some parts of your texts might disappear when exporting from FPD to Fusion 360. Text really is a 2D thing. When generating Gcode, you just want a single line/vector that your bit will follow. The milling depth is really a thing you setup in your CAM software. Same for cuts, drills, pockets... You would really need 3d CAD for some more complicated shapes like chamfer...

When i design front panel in Qcad, i tend to draw contours of cutouts, centers for drilled holes and texts on different layers.
In dxf2gcode, i can select shapes by layers, edit all the cut parameters (feedrate, depth...) and export one Gcode per layer.
Then i open them in bcnc, first i probe the surface, then I run all 3 gcodes one by one.

I drill round holes with a small bit first (1 mm) with the CNC and then i drill them to final dimension on the drill press. This way the CNC is not stressed too much and i can use it's precision to get my holes exactly where i want them.

Cheers

Thomas

 

[rob_gould]

Text in fusion 360 is a pain.

Using the native text tool doesn't work that well.

Importing text as a dxf or svg comes with its own problems.  I've been round the loop with this more than once for the work I do.

Unless you want something very simple, the best option is to prepare your text in another piece of software, get it to be the right size and in the right place in relation to your front panel, save it as dxf and then import the dxf onto the face of your extruded front panel body in fusion 360.

If this isn't adequately clear, let me know.

 

[substitute]

Unless you want something very simple, the best option is to prepare your text in another piece of software, get it to be the right size and in the right place in relation to your front panel, save it as dxf and then import the dxf onto the face of your extruded front panel body in fusion 360.

If this isn't adequately clear, let me know.

Mostly clear. Let's use Front Panel Designer as an example for generating our text DXF layer. I tried something similar to what you describe, made an extruded rectangle in 360, imported a dxf file and tried to extrude the text down into the body. I forget what went wrong but it didn't work. You know how in 360 when you hover over an element it turns black? Only bits of the text turn black and respond to commands, for instance the round part of the letter R or just one line in a T. Really strange behavior.

What do you mean about Python? I've used dxf2gcode for quite a while and never had to deal with python (or any scripting language).

Wild, is there a place to download a normal disk image/installer for dfx2gcode? When I searched for it this is what I found...
https://sourceforge.net/p/dxf2gcode/wiki/Installation/

The installation instructions are this...
Note(1): It is recommended to install python dependencies using 'pip' tool.
    $ ./make_tr.py
        If 'lrelease' is not on the PATH use something like the following:
        $ PATH=$PATH:/usr/local/Cellar/qt/5.11.1/bin ./make_tr.py
    $ ./make_py_uic.py
    $ ./st-setup.py py2app # builds standalone application

    To launch application use either:
        $ open dist/dxf2gcode.app
    or
        $ ./dist/dxf2gcode.app/Contents/MacOS/dxf2gcode

    It is still untested but in order to build dxf2gcode.pkg use the following:
    $ productbuild  --component dist/dxf2gcode.app /Applications dist/dxf2gcode.pkg



Greek to me. Thank you for the additional information about bits etc. That's helpful.

 

[totoxraymond]

which OS do you use?

i use a build for windows that might be outdated but worked well for me.

https://sourceforge.net/projects/dxf2gcode/files/DXF2GCODE-2017.09.25-win32.msi/download?use_mirror=netix

 

[rob_gould]

Ah, ok.  I think I understand. You don't need to extrude the text down into the face of the object at the design stage.

When you place your DXF onto the face of the object, at that point you've finished in the 'Design' section of Fusion360 and you move to the 'Manufacture' section.

In the Manufacture section, you can choose to 'engrave' from the same 2d operation menu as you choose pocket, contour etc and then select the  lines of your DXF file to specify what will be engraved.

 

[rob_gould]

A thought occurs to me....

Does Front Panel Designer only create single line text? I have a feeling that when I used it a long time ago, that was the case.

Fusion360 doesn't handle single line text very well because you can't select it for engraving. There's another 2d operation which can select it, but I recall that it's a bit of a pain.

I use illustrator to create my designs and save them as DXF, but I believe that inkscape will achieve the same thing for free if you don't have illustrator.

 

[substitute]

A thought occurs to me....

Rob, that really explains a lot, thank you. I had figured out some of this last night and was beginning to suspect that the bit about extruding the text was a mistake. And yes FPD appears to be using single line text.

I recently switched from illustrator to Affinity Designer (cost), it's a great program but it doesn't export DXF. Last night I made some progress exporting some graphics as SVG and bringing them into 360 as a layer on top of a body. The graphics were of a dial scale, the numbers behaved nicely, but the indicator lines wouldn't engrave (there's that line issue again). I was able to figure out that the 2D contour function can work for generating tool paths around a line but didn't get too deep into experimenting with it.

How do you handle line work? For instance say you had a vertical line in Illustrator with a 1 pt stroke, is there a function something like "convert to shape"?

 

[ruffrecords]

A thought occurs to me....

Does Front Panel Designer only create single line text? I have a feeling that when I used it a long time ago, that was the case.

When you say 'single line text' do you mean text on one line rather than on several or do you mean text that is engraved as a single unbroken line?

FPD  will do multiple lines of text but the engraving cost is still worked out on a per character basis.

FPD has a number if 'single stroke' fonts that contain characters that can be engraved as a single line. These are the easiest and cheapest to engrave but also the simplest. More complex fonts with lines of varying thickness for example needs a multiple stroke font. Either way, if you want FPD to engrave it  it has to be an engrave able font. FPB itself contains a list of such fonts.


Cheers

ian

 

[totoxraymond]

I think we were talking about single stroke fonts.

I never succeeded in engraving a multiple stroke font with my cnc, it always get messy. But i guess there's a way to do it.

 

[rob_gould]

I'm typing this on my phone so I'm typing from memory. Later I can turn my laptop on and take some screenshots if necessary

When using the engrave  tool, fusion 360 will automatically calculate the depth of cut etc based on the width of the line being engraved. That's why you can't engrave the single line text from fpd - the lines are too thin.

I also forgot to mention before that fusion won't let you use the engrave tool unless you're using a v bit. Again, this makes sense when you think that fusion works out how deep to make each cut to correctly engrave your text or graphic - the depth of cut is not something you can choose in the same way that you would if you were cutting a pocket, for example.

The other choice is to use the 'slot' operation. With this operations you can select single lines, and then the settings on the toolpath and the tool determine how the text will look. So if you use a 1mm bit for example, your lines will be 1mm wide.  You also manually set the depth of cut, so starting at 0.5mm or less is a good starting point probably.

So the Slot operation is kind of being misused in this context, but it can be made to work.

There are plenty of videos on YouTube about all this. Some are better than others, but it's what I used to learn plus a lot of experimentation and a good deal of cursing

As I say, I'm typing from memory so take this with a pinch of salt. I can check on fusion later if you need more detailed info on a specific bit.

 

[substitute]

When you say 'single line text' do you mean text on one line rather than on several or do you mean text that is engraved as a single unbroken line?

Text that is engraved as a single unbroken line.

When using the engrave  tool, fusion 360 will automatically calculate the depth of cut etc based on the width of the line being engraved. That's why you can't engrave the single line text from fpd - the lines are too thin.

AH HA! This was a really confusing point for me as some CAD/CAM platforms seem to require using single line text. I had figured out the bit about needing to specify a v-bit to get the engraving function to work, 360's built in library doesn't have one but I installed the amana library and can now get text created within 360 to simulate engrave paths. Thanks for the tip on the slot operation, I'm sure that'll be useful for something.

There are plenty of videos on YouTube about all this. Some are better than others, but it's what I used to learn plus a lot of experimentation and a good deal of cursing

I've been watching lots of youtube videos, I'm really surprised I haven't found anyone going over the details of milling a 19" rack, 500, or synth panel. I would have guessed it'd be a pretty popular use for home cnc. I've already cursed at my computer an extraordinary amount just getting to know the software I can only imagine the future frustration I may face.

 

[totoxraymond]

don't worry, things can get a bit frustrating but when you have your first panel done, it's a great feeling.

I can't tell how stupid i felt when i realised after several failures at engraving that my  z axis step/cm setting was wrong in grbl. Therefore, all my depths were wrong...

Make sure you buy a few cheap Al sheets at your local store to experiment. this way you won't throw away you're quite expensive anodised panels.

 

[rob_gould]

Text that is engraved as a single unbroken line.

AH HA! This was a really confusing point for me as some CAD/CAM platforms seem to require using single line text. I had figured out the bit about needing to specify a v-bit to get the engraving function to work, 360's built in library doesn't have one but I installed the amana library and can now get text created within 360 to simulate engrave paths. Thanks for the tip on the slot operation, I'm sure that'll be useful for something.

I've been watching lots of youtube videos, I'm really surprised I haven't found anyone going over the details of milling a 19" rack, 500, or synth panel. I would have guessed it'd be a pretty popular use for home cnc. I've already cursed at my computer an extraordinary amount just getting to know the software I can only imagine the future frustration I may face.

It sounds like you've pretty much cracked it now.  Now the fun begins 

 

[substitute]

Thanks guys, I think it's time to just order a machine and start messing around (with scrap material of course).

 

[abbey road d enfer]

Then i open them in bcnc, first i probe the surface,

How do you probe the surface? There are plug-ins that map the surface by probing every half-inch or so, is it what you're using?

 

[totoxraymond]

Bcnc has this probing option included.

I mount a microswitch in place of the bit (i'm using a 3d printed bracket for that). Setup in bcnc is pretty straightforward, it will detect the margins of your gcode, then you set the number of points, zero the machine and from this point the software handles everything on its own.

Once you have a defined map, bcnc will automatically compensate the milling depth while running.

You then only have to set the z=0 for each tool. I keep the same map as long as i don't move the piece.