OrCAD Layout - good ground

Hello, I need to make all the unused area on PCB into ground (I have only two layers - top and bottom). So, there should be paths for whatever connections there are, and and there would be space between those paths and ground (layer?). Of course, some components are connected to the ground anyway, so they way I layed them out, they form the area which should be ground only (i.e. no other paths). I do not know terminology well, so it might sound a bit awkward. Thanks in advance,

Vitaliy

Reply to
Vitaliy
Loading thread data ...

Copper pour?

Leon

Reply to
Leon

Set a copper pour zone around the area you want to have the copper ground plane, set the button that says to use the copper pour for connectivity, and then set no fill zones around areas where you don't want the copper to leak into.

-Chuck

Reply to
Chuck Harris

Thanks, I will try that tonight.

Reply to
Vitaliy

And while you are about it, use extra vias (or holes, or whatever the CAD allows) to stitch together the fills on the two sides, wherever one will fit. The idea is try to make the flood fill approximate to a continuous ground plane, rather than a set of disconnected leaves.

Paul Burke

Reply to
Paul Burke

************************************************************

If the PCB you are designing is going to be produced on a flow solder line

then you should take extra care when incorporating earth or power planes.

If your earth planes are large then you should fill them with a cross hatch fill and

ensure that any via's or component holes connected to the earth plane are designed as

thermal relief pads, otherwise the pads will wick and draw up solder and you will have

lots of solder bulges around the pads on the soldered side of the pcb.

John Law

Reply to
John Law

That reminds me of something that he will have to deal with, and that is, left to its own devices, the autorouter will route the ground wires, in addition to the ground plane. This will add extra wires through the thermal reliefs it automatically adds to ground pads. You have to tell the router not to route ground.

In the default condition, via's are covered with solder mask, so they don't need to be thermal releaved on the ground plane. In the default condition, all ground plane pins are already thermal releaved.

A hash ground plane is a nice idea if you can afford the leakage, usually on my RF projects, it is not an option.

Copper fills slow down the scrolling and refresh rate of the screen. You should leave the display copper fill option off, except when you specifically want to see copper pours.

-Chuck

Reply to
Chuck Harris

EasyPC must have a pretty good algorithm then. The fill scarcely slows things down, even on my increasingly- antique 800MHz system.

I often do turn them off, but that's just because they get in the way of seeing where the tracks go.

Paul Burke

Reply to
Paul Burke

I doubt that their algorithm is any better than Orcad's. Small boards are no problem. It becomes a problem when you do boards that are about one foot on a side.

-Chuck

Reply to
Chuck Harris

Orcad's V10.x release broke the copper fill display in "fast fill" mode. Now fast fill is extremely slow fill when zoomed in. Much faster to use skeleton or normal fill modes. I had a talk with a EDA rep and he was clueless. Orcad's new policy of doing programming in India has caused lots of problems in the new releases.

--
Mark
Reply to
qrk

I just tried copper pour on a 1 ft square board with Pulsonix, it was almost instantaneous. I do have a 64-bit dual-core Athlon with 1 Gbyte of RAM, though.

Reply to
Leon

In general I've found that the older a piece of PCB software is, the slower scrolling is! ...with notable exceptions for things like ORCAD 386/SDT, of course. Similarly, I'm actually surprised that most PCB packages still even have the option of drawing in "outline mode" -- I was told that came about primarily due to the slow speed of now-ancient computers and graphics terminals.

Reply to
Joel Kolstad

A good part of this performance problem is the older packages do their graphics with 16 bit I/O data transfers, while the newer packages use the most efficient block transfer methods that are available on new hardware.

-Chuck

Reply to
Chuck Harris

Thank you all for your replies. They board I am doing is going to be relatively small size (max 1.5'' by 3.5''). I am not exactly sure what flow solder line is. I added copper pour.

  1. I would like to stich together the planes in the corners of the board, however, I ran into problem. "Free vias must attached to the net". For now, now mounting holes are planned. Does that mean I can not use free vias to stich the planes in the corner? Here are the qoutes from Orcad's help: "Free vias must have a net attachment, though they do not appear in a schematic or netlist. ...You can use free vias for special purposes, such as zero length fanouts of ball-grid array components and the "stitching" of plane layers. ..."

  1. Is it ok to use free vias under surface mountable components?

  2. When free via is created, does it mean that physically there will be a hole in the board, which would need to be filled up by copper?

Thanks in advance, Vitaliy

Reply to
Vitaliy

Free vias are manually placed vias that take a little effort to delete, thus deleting traces to a free via will not remove the free via. Free vias must have a net associated with them. Double clicking on the free via in a routing mode will bring up a dialog box where you can change parameters of your free via.

If you want to join planes in the corner of the board, you can use your mounting holes to do this if you don't mind connecting your ground plane to chassis. Simply define the holes in your schematic as a one-pin device and connect them to ground.

If you want to use free vias to stitch the planes, then route out a ground trace from some pin and insert a free via at the end of the trace. Delete the trace to your free via and move it to the desired location. You can copy this free via and place the copies else where.

--
Mark
Reply to
qrk
2) It is OK to use free via's under SMT components if you are getting the board manufactured at a PCB house where they plate the holes to connect the two sides, nice and flat. If however you are routing the PCB on a prototype milling machine that uses conductive glue to plug the vias it can leave a little 'tent' of glue which may interfere with placing the component flat on the PCB, likewise if you are actually hand-soldering the via's with wire (yes some people still do this!).

3) Yes there will be a hole. It does not need to be 'filled' per se, but a PCB manufacturer will plate it with copper creating a barrel shape, if the diameter is big enough you will be able to look through it. If you are using conductive glue: fill it, hand-soldering: fill-it.

Alan

formatting link

Reply to
electronic-eng.com

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.