Future of stand-alone Eagle on Linux

[Karel]

https://forums.autodesk.com/t5/eagle-forum/is-eagle-retired/td-p/9516332

Look how Matt is trying to avoid the hot potato...

[KE5FX]

That's the thing about credibility.  It's hard to get it back once you lose it.

[Monkeh]

It has no future. That's been the case since Autodesk got involved, I'm afraid.

[Quarlo Klobrigney]

"That's been the case since Autodesk got involved, I'm afraid..."

[ataradov]

It is pretty obvious that Eagle is done for. Thankfully KiCad is actually improving rapidly.

[ebastler]

Look how Matt is trying to avoid the hot potato...

When Matt states,

the fact that we have added the PCB design capabilities into Fusion is an indication that at some stage we may tip the balance in favor of one platform,

that seems clear enough. To paraphrase: "Yes, of course we plan to eventually discontinue Eagle as a stand-alone product and force Fusion down your throat".

[macegr]

When Matt says "we currently have no plans to" it has historically meant "we are 100% going to do it and I want people to keep spending money instead of getting upset right now"

[madires]

Anyone surprised? Based on Autodesk's history it's pretty clear that this is going to happen at some point. The only open question is at which time exactly.

[jaycee]

My opinion on this is that Autodesk are a lying bunch of f**ks who have ruined a good product. Screw them. I will happily use my cracked version of Eagle 7.6.0 which does everything I want, and runs where I want without Autodesk interfering.

[jpanhalt]

@jaycee
I realize this is an old thread but agree with that sentiment.  I use 7.2 and 7.7 (purchased).  I still use the classic icons.  As for the enhancements I have read about, I would probably not use them. 

The one thing I have needed is support for plated slots.  OshPark has a modified CAM that does that.  I asked JLCPCB whether it would work for them in late 2019, and was told they would get back to me.  Hasn't happened yet. 

Of course, it also doesn't have workable 3D, but I don't need that either.

[ebastler]

The one thing I have needed is support for plated slots.  OshPark has a modified CAM that does that.  I asked JLCPCB whether it would work for them in late 2019, and was told they would get back to me.  Hasn't happened yet. 

Umm, you mean plated slots like for the mini USB and the RS-232 (mini DIN) jacks in the photo here? That board was designed with Eagle 7.6, and made by JLCPCB.

If I recall correctly, all it takes is a regular oval through-hole pad with a round drill, plus a slot defined in the milling layer at the same position. Both are part of the footprint in the library, so no special trickery is involved when invoking the part.

[oPossum]

If I recall correctly, all it takes is a regular oval through-hole pad with a round drill, plus a slot defined in the milling layer at the same position. Both are part of the footprint in the library, so no special trickery is involved when invoking the part.

That is what I do for JLC and OSHPARK.

JLC says to leave a note if you have plated slots. Don't do that - it just confuses them.

[jpanhalt]

@ebastler

Thank you for the example.

Yes, that is what I wanted.  JLCPCB and I had about 2 or 3 email exchanges.  Here is what I submitted to JLCPCB in March 2020 and got no reply:

2)  Plated through slots are more difficult, as my version of Eagle does not have a specific way to do it.  Oshpark and Eagle suggest using a “long pad” of the proper dimensions.  The drill dimension for the hole is then used to draw a slot of the proper length using the Milling layer (#46).  Alternatively, Eagle suggests building the PTH slot from separate layers:  2 Vias (one at either end), Milling (#46), Top (#1), Bottom (#16), t-Stop (#29), and b-Stop(#30).  Which of those two ways do you  prefer, or is there another method?

What you did sounds identical to the first option that I describe.  Did you submit the .brd file or the Gerbers?   For Gerbers, JLCPCB asked for a layer that Eagle did not make.  I went ahead and ordered from Oshpark with Gerbers, since I used its edited CAM processor.  I order PCB's so rarely that the price difference doesn't matter as much as the color.  I like red instead of purple.    Also, Dan (OshPark) is a great help, so I tend to send my business his way, but I would still like to know how to use JLCPCB is an option.



 

[ataradov]

That is what I do for JLC and OSHPARK.

Can you share that footprint?

Not having slots is one of the things stopping me from going USB C. I want to try that with AllPcb and PCBWay too.

[oPossum]

That is what I do for JLC and OSHPARK.

Can you share that footprint?

Not having slots is one of the things stopping me from going USB C. I want to try that with AllPcb and PCBWay too.

Sure. Eagle library attached.

[jpanhalt]

@oPossum

It appears you use the dimension layer for the slot, and because there is copper on both sides, it gets plated.

If that is correct, it is logical and easy.

EDIT:  Are you using version 7.x or something later?

[oPossum]

A zero width line intersecting copper seem to be the key to getting plated holes. I put the slot on the dimension layer because it is already included in the CAM configuration. It doesn't matter what layer it is on as long as it ends up in the proper gerber file with the board outline.

Eagle 7.7.0

[jpanhalt]

Now, that is interesting.  Autodesk (and earlier Eagle) defines the dimension layer as:

Layer 20: Dimension
The Dimension layer has several purposes, the first of which is to specify the outline of your board. Secondarily, you can also use this layer in your design rules to keep copper pours away from the edge of your PCB.

In fact, as I recall, there were instructions not to use dimension though copper layers -- hence the clearance between copper and PCB edge.  LIke I said earlier, logically a structure in the Dimension layer through a pad should give a plated slot.

Thank you for showing that it really works.

John 

[oPossum]

It does keep copper pour away from the slot and there are some DRC errors that must be approved. Putting the slot on the milling layer is probably a better way to do it. I may try that next time.

[jpanhalt]

Were the slots made here:



done the same way?  They look connected to the GND pour, which is probably what one usually wants.

If they are not connected, then I will also use the milling layer.  The advantage is that the Dimension layer is what I believe JLCPCB wants and, as you say, it is already include in that CAM file.

[ebastler]

I just checked my design file, and I did use the milling layer to define the slots. This has worked well for unconnected pads, pads connected to signal traces, as well as pads connected to the GND pour via thermals. Eagle keeps the copper pour away from the pad anyway -- no need to keep it away from the slot by (ab?)using the dimension layer.

I had sent Gerber files to JLCPCB, not the Eagle board files, by the way.

[jpanhalt]

Here is a macro shot of the board I sent off to Oshpark using the Milling layer, named GND, and thermals turned off:

" alt="" class="bbc_img" />

Those slots are connected to the ground pour.  I am really bad at macros currently.  Maybe I should do an update from my cheap, digital microscope.

[ebastler]

Those slots are connected to the ground pour. 

So did you place the slots right into the ground pour polygon? In that case I would expect them to be connected as shown.

Or are there pads surrounding the slots? In that case, I would expect the pads (and hence the slots inside them) to either be totally isolated from the ground pour, if the pads are not defined as GND pads. Or they should be connected to the ground pour via thermals, if they are GND pads.

That's how Eagle should define the copper layer if there were no slots present. And nothing should change by adding the slots. And in my experience, that is how Eagle does indeed behave. -- Or am I missing something here?

[jpanhalt]

I followed the old Eagle/Oshpark directions.  It's a long pad (hole in center), drill adjusted to what I wanted, and milled to the length I wanted at same width as diameter of the hole.  Of course, the pad was named "GND" so it would be included in the pour.

That design is in the library file (package), so I didn't need to go through those machinations on the board.  I have other plated slots for attachment clips and passages done the same way, i.e., as devices, or they can be drawn on the board.

[ebastler]

Of course, the pad was named "GND" so it would be included in the pour.

Then you had the "Thermals" option un-selected in the definition of the ground polygon, right? That would cause the pad to be fully connected to the ground plane (which makes it hard to solder by hand).

But that has nothing to do with the presence of the slot, or its absence. If you want the pad to be separated from the ground plance, and connected only via discrete traces, I would recommend doing that via the "Thermals" option, not via a slot in the dimension layer.