Platform forum

Internal Plane

mulfycrowh , 01-31-2019, 04:26 PM
Hi everybody,

An internal plane is assigned to a single net name.
How do you set the number of internal planes on a project ?
Thanks a lot.
robertferanec , 02-03-2019, 10:12 AM
You need to go to stackup manager. Maybe this will help: https://www.fedevel.com/welldoneblog...e-new-old-way/
mulfycrowh , 02-03-2019, 03:33 PM
Thanks Robert. I already watched this video but I didn't find how you set the number of the internal planes. Let's take an example. We have a schematic with 3 power supplies, digital GND, analog GND. Very often you assign the planes to GND. But in this case, do you assign internal planes to DGND, AGND and the 3 power supplies ?
Paul van Avesaath , 02-05-2019, 12:51 AM
pretty straight forward.. same in 17 as in 18
mulfycrowh , 02-05-2019, 01:42 AM
Thanks for reply. Could you please explain a little bit. How many internal planes do you set ? And how do you assign them ?
Paul van Avesaath , 02-05-2019, 02:09 AM
that all depends on how many you need which can vary between projects.. . just be sure to keep it symmetrical.. let say you need a 6 layer board.. than it could be toplayer/internal plane1/mid layer 1/ midlayer 2/Internal plane 2/ Bottom layer.. or toplayer / midlayer 1/ internal plane 1 / internal plane 2/ midlayer 2 / bottom layer..

to assign a plane go into the pcb editor (to your pcb) select the internal plane.. double click anywhere on you plane and select the net you want it to be.

good luck
mulfycrowh , 02-05-2019, 02:34 AM
sorry but I gave an example About 3 power supplies with DGND and AGND. Could you please share how to set the internal planes ?
Paul van Avesaath , 02-05-2019, 02:58 AM
I told you how to add planes, gave an example of a layerstack , and how to set them to a specific net.
you need to give a lot more information before you can ask something like this..

as an example, where do you need the DGND and AGND to be.. maybe they can be on the same internal plane?..
same goes for your 3 power supplies.. maybe they can go on the same internal plane..

so that would give you a simple 4 layer board.. (top / int1 / int2 / bottom)

you do not need to use a full plane for each...you can draw lines (command: place line) on an internal plane, everything you draw on there is inverse.. (so what you draw will be come no copper)
see attached image.

so if you draw a closed box of any shape and double click inside the box you can assign a box to a different net. the highlighted area is now a seperate copper area inside you internal plane

so you can divide your internal plane to be DGND and AGND and you other plane to multiple power supply .

hope this clears something up for you..

mulfycrowh , 02-06-2019, 02:58 AM
Hello everyone,

Thanks for reply.
Could we just forget Altium a few minutes.
What is the main purpose of the internal planes ? Is it shielding ?

Paul van Avesaath , 02-06-2019, 06:10 AM
its for distributing power / gnd over a large area.
If you want impedance, then is is used as reference plane.
it has a very low impedance itself so for large currents is is much better than traces.
also in production it gives regidity and stability
Paul van Avesaath , 02-06-2019, 07:47 AM
also if you look at this from an Signal intergrety point of view.. you need a proper GND plane if you want the current retun path to run underneath the trace.. so when going high speed.. you need planes.. also like you suggest for shielding
mulfycrowh , 02-24-2019, 01:43 AM
Coming back to you.
Hello everyone !

Well my suggestion for my 4 layers PCB is:

Top Overlay
Top Solder
Top Layer (dedicated to high speed tracks)
Dielectric Prepreg
Inner layer 1 >>> GND (in fact AGND + DGND) used to act as a shielding for high speed tracks
Dielectric Core (FR4)
Inner Layer 2 >>> VCC
Dielectric Prepreg
Bottom Layer (dedicated to low speed tracks)
Bottom Solder
Bottom Overlay

First question:

As I already dedicated layers to GND and VCC, do I need additional internal planes ?

Second question

Is the stackup correct ?

Thank you !

Paul van Avesaath , 02-24-2019, 03:16 PM
seems ok to me..
just keep it symmetrical so same distance between top and interplane1 as for bottom to internal plane2.. use the inner layer between the two internal planes to fill the gap to your pcb thickness.. you do not need any other planes as far as I can see now.. but i dont know what you are designing so it is hard to comment on that..
mulfycrowh , 02-24-2019, 03:43 PM
Thanks for reply.
The board uses RS485 link. So we use 120 ohm impedance.
So it means that you add internal planes in addition to both inner layers ?
Paul van Avesaath , 02-25-2019, 12:21 PM
no you do not need this.. for RS485 you can get away with no impedance.. dont worry about it.. if yo were desinging a 10G link then i would be more concerned.. but you can use your stackup with no issues at all! good luck!
mulfycrowh , 02-27-2019, 06:16 AM
Thanks for reply.
I know that this development doesn't imply high speed signals.
I would like to make it to prepare the next developments that are far much complicated.
What disturbs me is that I asked the PCB manufacturer to compute the impedances (50 and 120 Ohm for this first project) and they told us they do not perform any impedance calculations.
They suggest us to use the following free calculators to do it:


Paul van Avesaath , 02-27-2019, 06:36 AM
I use the PCB saturn tool for basic impedance caluclations. it gives you a good indication, but if you need 5% or 10% accuracy in your design the manufacturer should be able to control the impedance.. because they have all the exact numbers and material specs that might deviate from normal numbers.. you pay for this option it is not for free because they have to do extra TDR measurements after production on the test coupons they produce in the same batch.. also they might have to scrap a batch because they did not meet the spec.. so they have risk of less yield per batch.

There is a difference here though..
If you are talking to the manufacturer of the pcb (e.g. Fineline global) then they should be able to suggest a stackup and impedance report, (if not they choose a different one).
If you are talking to you EMS then i can imagine you get an answer like that because they get the PCB and only place components on it.

if you are ordering a PCB through a EMS then they should be able to forward your request or bring you into contact with the correct persons.

hope this helps..
robertferanec , 03-01-2019, 02:19 AM
I asked the PCB manufacturer to compute the impedances (50 and 120 Ohm for this first project) and they told us they do not perform any impedance calculations.
- If you need impedance controlled boards, do not use this PCB manufacturer. Every serious PCB manufacturer will provide you with the calculations. Of course, there are some factors - as they need to spend their time on the calculations, they would like to be sure, they will manufacture your PCB. Otherwise they may not be very keen to help.

Other option could be to check PCB manufacturer websites. Some PCB manufacturers may have "default" stackups with all the impedances calculated. For example try to have a look at Sierra circuits - they are expensive, but maybe their calculator could help you (I used their calculator long time ago, but I think their calculator should give you accurate numbers based on materials and their PCB manufacturing process): https://www.protoexpress.com/hdi/hdi-tools.jsp
mulfycrowh , 03-01-2019, 02:27 AM
I totally agree with you.
I have a RS 485 link with a length of about 1m40. The impedance has to be 120 Ohm.
robertferanec , 03-01-2019, 05:30 AM
I have a RS 485 link with a length of about 1m40. The impedance has to be 120 Ohm.
For RS485 it may not be so critical. Usually what I do is that I keep the transceiver very close to the connector and then even if these short tracks (the tracks between transceiver and connector) are not controlled impedance, it is fine.
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?