Solid ground plane with ORCAD LAYOUT

D

David

Guest
Hi everyone!

I'm having problems with Orcad Layout. I've desgned a PCB for my
company and I've sent the GERBER files to the factory. But the factory
operator said me that the ground planes I've created on my design
aren't solid planes and they must be solid planes.

My idea was to use all the unused PCB surface to make the ground
tracks bigger, so they take all the space available where there are
any tracks. Therefore I've place a big copper pour obstacle associated
to the ground net. The result seems to be really good, I mean I can
see a lot of copper areas going around the tracks.

But the factory guy said that, actually, the copper obstacles are made
of thousands of little tracks (about 75000 tracks!!). So they just see
a lot of tracks instead of a real copper area despite it seems a
homogeneous area. But this is a problem for the PCB's machine.

Somehow I needto tell Orcad that the copper pour must be a continuous
and homogeneous area.

Could you help me? I need to work out with this problem now!

Regards
 
On Wed, 8 Oct 2008 08:09:13 -0700 (PDT), David <dgvalde@gmail.com>
wrote:

Hi everyone!

I'm having problems with Orcad Layout. I've desgned a PCB for my
company and I've sent the GERBER files to the factory. But the factory
operator said me that the ground planes I've created on my design
aren't solid planes and they must be solid planes.

My idea was to use all the unused PCB surface to make the ground
tracks bigger, so they take all the space available where there are
any tracks. Therefore I've place a big copper pour obstacle associated
to the ground net. The result seems to be really good, I mean I can
see a lot of copper areas going around the tracks.

But the factory guy said that, actually, the copper obstacles are made
of thousands of little tracks (about 75000 tracks!!). So they just see
a lot of tracks instead of a real copper area despite it seems a
homogeneous area. But this is a problem for the PCB's machine.

Somehow I needto tell Orcad that the copper pour must be a continuous
and homogeneous area.

Could you help me? I need to work out with this problem now!

Regards
Click to expand...
The copper pours are normally made up of many draw lines. You can
control the number of lines by specifying the width of the line in the
obstacle dialog box. Somewhere in the 5 to 10 mil width is good. If
your design isn't crowded, then you can use a wider width like 20
mils.

Also, be sure that your plane is set to solid. There are other options
in the obstacle dialog which let you set hatched planes for copper
robber patterns.

You should be able to preview what Gerber data looks like with
GerbTool which comes packaged with certain versions of Layout
(Tools|GerbTool). If you don't have GerbTool, download one of the free
Gerber viewers to see what your board really looks like. If fact, you
should always view your Gerber data before sending it out to be sure
that the Gerber data matches what you think you should have.

Be sure to set your copper pour preferences in Options|User
Preferences to Enable copper pour and use pours for connectivity. Fast
mode and skeleton display should be turned off. Layout will bugger the
copper pours if copper preferences aren't set up correctly.
 
David,
The key question here, why is the "factory guy" telling you what he is
telling you? I think there may be some confusion about his comments. You are
interpretting it that the copper polygon should be solid (not drawn from
individual lines) but I would bet he is calling for a solid ground plane
within the board (a multilayer board design). What you have described about
your design is quite normal for a lot of designs, designs use a poured
polygon GND flooded over the unused areas of the design quite often. And the
multitude of individual lines making up that polygon pour is quite normal
also.

But why is the factory telling you what to do? Just fishing here because
the relationship sounds a little funny the way that you have stated it in
such limited detail.
Do your GND connections make connections to all GND points without
breaks? Do your OrCAD DRC checks report any incomplete routes/connections?

Do you have any controlled impedance lines called out? That could be a
problem causing such a request from the factory guy. You can't have
controlled impedance without a contiguous associated plane directly below or
above your trace. If you have controlled impedance in this design then you
obviously don't understand the requirements for impedance controlled lines
and the factory guy knows you need a contiguous internal plane to achieve
the impedance control for those lines.

--
Sincerely,
Brad Velander.

"David" <dgvalde@gmail.com> wrote in message
news:cd2faf90-a1ab-4e06-8ad2-905ac91c3d81@p10g2000prf.googlegroups.com...
Hi everyone!

I'm having problems with Orcad Layout. I've desgned a PCB for my
company and I've sent the GERBER files to the factory. But the factory
operator said me that the ground planes I've created on my design
aren't solid planes and they must be solid planes.

My idea was to use all the unused PCB surface to make the ground
tracks bigger, so they take all the space available where there are
any tracks. Therefore I've place a big copper pour obstacle associated
to the ground net. The result seems to be really good, I mean I can
see a lot of copper areas going around the tracks.

But the factory guy said that, actually, the copper obstacles are made
of thousands of little tracks (about 75000 tracks!!). So they just see
a lot of tracks instead of a real copper area despite it seems a
homogeneous area. But this is a problem for the PCB's machine.

Somehow I needto tell Orcad that the copper pour must be a continuous
and homogeneous area.

Could you help me? I need to work out with this problem now!

Regards
Click to expand...
 
David

Another possibility is the kind of gerber's that you have created. the
gerber format is basically "drag shape x from point a to point b". x
can be defined in the file or in a seperate file depending on gerber
type.

Orcad is really irritating in not creating a sub-directory for output
files, you may have not sent him the "x" definitions.

Colin
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top