OrCAD Layout - good ground

V

Vitaliy

Guest
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
 
Vitaliy wrote:
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.
Click to expand...
Copper pour?

Leon
 
Vitaliy wrote:
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

Set a copper pour zone around the area you want to have the copper ground
Click to expand...
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
 
Chuck Harris wrote:
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.
Click to expand...
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
 
"Paul Burke" <paul@scazon.com> wrote in message
news:44b9glF19npbU2@individual.net...
Chuck Harris wrote:

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.

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
Click to expand...
************************************************************


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
 
John Law wrote:
"Paul Burke" <paul@scazon.com> wrote in message
news:44b9glF19npbU2@individual.net...
Chuck Harris wrote:
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.
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

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


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
Click to expand...
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
 
Chuck Harris wrote:

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.
Click to expand...
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
 
Paul Burke wrote:
Chuck Harris wrote:

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.

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
Click to expand...
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
 
On Wed, 01 Feb 2006 14:08:32 -0500, Chuck Harris
<cf-NO-SPAM-harris@erols.com> wrote:

Paul Burke wrote:
Chuck Harris wrote:

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.

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

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
Click to expand...
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
 
Chuck Harris wrote:
Paul Burke wrote:
Chuck Harris wrote:

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.

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

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.
Click to expand...
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.
 
"Leon" <leon_heller@hotmail.com> wrote in message
news:1138882351.904705.236490@z14g2000cwz.googlegroups.com...
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.
Click to expand...
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.
 
Joel Kolstad wrote:
"Leon" <leon_heller@hotmail.com> wrote in message
news:1138882351.904705.236490@z14g2000cwz.googlegroups.com...
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.

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.
Click to expand...
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
 
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. ..."

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

3. 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
 
On 3 Feb 2006 10:24:31 -0800, "Vitaliy" <vmykhayl@ee.ryerson.ca>
wrote:

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. ..."

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

3. 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
Click to expand...
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
 
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
www.electronic-eng.com
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top