EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => Eagle => Topic started by: Faringdon on June 11, 2022, 04:47:48 pm
-
Hi,
I am just coming to the end of a 2kW Offline SMPS in Eagle Pro 7.4.0.
I have used loads of copper pours. It takes some 5 seconds to re-pour the copper pours every time they are un-poured.
I do this a lot and it takes lots of time.
Is there any way i can kind of "temporarily shelve " the copper pours so that the board is quicker to work on?
-
I am just coming to the end of a 2kW Offline SMPS in Eagle Pro 7.4.0.
I have used loads of copper pours. It takes some 5 seconds to re-pour the copper pours every time they are un-poured....
Have you tried increasing the pours' Wire Width?
-
Agreed on changing the width. My most recent board ( about 50mm x80mm) has just 2 pours 0.006 width and 0.12 isolate, and it fills almost instantly. Many years ago, I used the smallest width to get a logo (attached). The place I submitted to said the pour lines were too small and rejected it. For DIY using a photoresist, it worked fine. You may need a small width for pours into small gaps. You can sometimes work around that by putting a trace or separate pour and name it the same, if there are not too many. But, that would be my fallback solution.
-
Thanks, i have loads of pours......and whenever a component has a PTH pad on the bottom, and no trace to it on the bottom...i put a pour over it, so its more fixed if i have to desolder it.
I just wish there was some way i could copy all the pours to another file, and then work on the board...and then bring all the pours back later....so it wasnt so slow every time i hit ratsnest.
-
Thanks, i have loads of pours......and whenever a component has a PTH pad on the bottom, and no trace to it on the bottom...i put a pour over it, so its more fixed if i have to desolder it.
I just wish there was some way i could copy all the pours to another file, and then work on the board...and then bring all the pours back later....so it wasnt so slow every time i hit ratsnest.
As a longtime user, I don't understand that problem The bottom pad of as TH component that is not part of the pour signal should not require its separate pour to isolate it. For example, if the pour is "GND" anything that is not GND will be excluded from the pour.
Since you are using Eagle 7.x, if you post a snippet picture and the .brd file, we may understand the problem better. I believe Jorge is still at Autodesk. He is the #1 expert on Eagle, IMHO. Have you posted the problem there? Maybe, post it here first to see if the answer is obvious.
John
-
use "set poly off" in the commandline.
than "ripup @;"
the next ratsnest works without polygone.
to see the polygone again: "set poly on"
followed with a ratsnest-command.
If you don't want to type the commands: create 3 menu-buttons for these commands. type:
MENU 'ripup @;' 'Poly ON: set poly on' 'Poly OFF: set poly off' ENTER
-
Thanks, i have loads of pours......and whenever a component has a PTH pad on the bottom, and no trace to it on the bottom...i put a pour over it, so its more fixed if i have to desolder it.
I don't quite understand what you are doing there, but you might be misunderstanding (or abusing) the pour feature.
Do you mean that you use a local pour, set to the signal on the pad, to essentially make a larger pad? If so, I recommend against it. That's asking for trouble if you have to change the layout, e.g. move components around. If you really want larger pads, you should edit the component footprint.
But placing larger pads just to make the pads more robust during the testing & debugging phase seems a bit over the top for my taste. Plated-through, double-sided pads hold up quite well in my experience, even on PCBs from the typical low-cost suppliers. How often do you expect to unsolder the components?
-
se "set poly off" in the commandline.
than "ripup @;"
the next ratsnest works without polygone.
to see the polygone again: "set poly on"
followed with a ratsnest-command.
If you don't want to type the commands: create 3 menu-buttons for these commands. type:
MENU 'ripup @;' 'Poly ON: set poly on' 'Poly OFF: set poly off' ENTER
Thankyou so much!....you are brilliant...utterly Brilliant !!!
....this will save so much time its not true...
I will come to other great points of others too....
-
I must admit i went on too far, editing the PCB , then fond it was too slow...which of the following woudl you say contributes to slowness in an Eagle Pro 7.4.0 layout.?...
1....Lots of tracking in "free angle" (ie not 90 degree or 45 degree)
2...Lots of copper pours
3.....Lots of copper pours with multiple "sides"...ie made of freely drawn "free angle" wire width.
-
I have not noticed any particular slowness by having non-45 degree angles for traces or irregular polygon pours.
Lots of pours will slow things down and particularly if the wire width is very small, e.g., 0.