multi-layer PCB design and ground free area in Altium  - Page 1
Forum section: electronics / general

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 09:40:41 am
content: Hello*updatedI have set 4 layer signal instead of (2 signal later+2 planes).now my problem is:I have some sensitive nets as follow:I can pour polygon around it without any problem (consider with 20 mil clearance)also I should put ground layer under this layer. but this area should be ground free! this is my problem bcoz the sensitive nets are on the top layer!

author: Psi
author_rank: Super Contributor
timestamp: November 21, 2017, 09:45:32 am
content: You can have the inner layers setup as power planes or as just another layer.Assuming you have them setup as generic layers,change to one of the inner layers and create a polygon pour. Select the area (all of pcb if you want) and then you can give it a net in the polygon pour properties window (double click on polygon to get it).You may also want to setup some polygon rules, you can have the clearance different for polygon pours etc.You can also lock a polygon pour if you want to avoid clicking on it by accidentor you can shelf it and restore layer,To create a area within a polygon pour where you don't want to fill, use the 'polygon pour cutout' object. Its in the menu somewhere. It just defines an area where a polygon is cutout and will not fillIf you have your inner layers setup as specific power planes then i'm not sure how you configure those.I've never bothered to use them in that mode. I prefer the flexibility of generic layers

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 10:01:29 am
content: Quote from: Psi on November 21, 2017, 09:45:32 amI'm wondered. when I put polygon and see the Layers, I don't see my Planes!

author: tautech
author_rank: Super Contributor
timestamp: November 21, 2017, 10:17:58 am
content: I haven't done one for a while but try single layer mode and assign the Net.I never routed the power Nets fully instead just to where a pour can get to them without breaking rules.

author: Psi
author_rank: Super Contributor
timestamp: November 21, 2017, 10:29:27 am
content: This is what i haveAlso, check your layer stack has inner layers and not inner planes

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 11:12:08 am
content: when I want to place a solid region, the planes are in the Layer list! but when I want to pour a polygon the plane layers are not in the Layer list!

author: tszaboo
author_rank: Super Contributor
timestamp: November 21, 2017, 11:16:09 am
content: Planes are inverted. Poligon pour is to connect things together. So it is contradicting the very function it supposed to do, that is why it is not there.

author: Psi
author_rank: Super Contributor
timestamp: November 21, 2017, 11:24:03 am
content: Yeah, it sounds like you have your layerstack setup for two layers and two planes, rather than just 4 layers.I've never used plane layers, so i dunno how you make it work.

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 01:04:16 pm
content: Quote from: Psi on November 21, 2017, 11:24:03 amQuote from: NANDBlog on November 21, 2017, 11:16:09 amYes, I have two Layers and two Planes! 2+2=4 what should I do?I can remove two planes, then add two Layers inside and set the inner layers as Ground and Power Planes.

author: tszaboo
author_rank: Super Contributor
timestamp: November 21, 2017, 01:10:17 pm
content: Quote from: xzswq21 on November 21, 2017, 01:04:16 pmPlease, first understand what is the difference between a plane and a layer.You just wrote: I remove the planes and add layers and set them to be planes.

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 01:14:37 pm
content: Quote from: NANDBlog on November 21, 2017, 01:10:17 pmdid you load a 4 layer PCB from Layer Stack Manager? I mean from default setting in Altium. it has 2 layers and 2 planes.I want to have 2 layers for signals and 2 layers for the ground and the power. what should I do?

author: tszaboo
author_rank: Super Contributor
timestamp: November 21, 2017, 01:18:30 pm
content: Quote from: xzswq21 on November 21, 2017, 01:14:37 pmQuote from: xzswq21 on November 21, 2017, 09:40:41 amSo you already have a ground and a power plane... Why do you want to do something, that you already have?

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 01:22:39 pm
content: Quote from: NANDBlog on November 21, 2017, 01:18:30 pmDearI have a ground and two power (+/5V). some Area of ground plane under High speed traces should be free. on the other hand I should have +/-5V separately at the power plane! like the top layer I could be able to edit and rout the power traces.

author: tszaboo
author_rank: Super Contributor
timestamp: November 21, 2017, 01:30:15 pm
content: You make cut-outs on a plane by placing a fill.You can divide a plane with lines and assign different nets to two parts of the plane.If you want traces in the inner layer, call it an inner layer, and not a plane. Yes you can delete a plane and add a layer instead.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 21, 2017, 02:27:13 pm
content: Planes are constructed out of negative space. When viewing the plane layer, you can select the plane region and assign a net to it. It will then connect automatically with any vias and THT pads of the same net (indicated by a thin "X"), and clearance all other nets. Both behaviors are governed by the plane rules. Plane rules are not as flexible as polygon rules.To make separate areas for routing your +5V and -5V nets, draw traces to outline their locations. When a closed shape is complete, select the plane regions and assign their nets accordingly.Tim

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 02:58:53 pm
content: Quote from: T3sl4co1l on November 21, 2017, 02:27:13 pmDearI have a sensitive area around an op-amp. under this area should be ground free.consider the op-amp is on the top layer.I pour a polygon around it with 20mil clearance. then I sent it to the ground layer. now I should convert this polygon into an cut-out area.... HOW should I convert it?

author: tszaboo
author_rank: Super Contributor
timestamp: November 21, 2017, 03:28:44 pm
content: Again: Dont use poligon pour, use solid region.

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 07:08:48 pm
content: Quote from: NANDBlog on November 21, 2017, 03:28:44 pmSolid Region is not similar to Polygon! I want to build a sensitive area. I could build it by polygon on the top layer. now How should I convert it to a solid region?

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 21, 2017, 07:55:27 pm
content: you see the sensitive nets below:all them are in the top layer.when I want to build a ground and power layers under this area, this area should be ground free and power free (clearance 20 mil )

author: Siwastaja
author_rank: Super Contributor
timestamp: November 22, 2017, 07:35:45 pm
content: If I understood correctly, you want to keep the top layer polygon ground pour further away than what you "normally" get (per your clearance rules), for whatever reason (I can't quite understand why, but let's not discuss that).For that purpose, I'd consider using "polygon pour cutout" feature. You can draw any shape you want, and the pour doesn't go inside that area.http://www.altium.com/documentation/17.0/display/ADES/PCB_Obj-PolygonPour((Polygon+Pour))_AD#!PolygonPour-PolygonPourCutoutThe same works for internal layers if you did them as standard "layers" & polygon pours on them, instead of using "planes".With planes, you need to just draw a polygon, fill, heck, even bunch of lines there if you so wish.I almost never use planes myself, because often I find I need to place a trace anyway on the inner layers, even if they are "mostly" planes. So then you just need to do them as "layers". Easier to think about when all the actual PCB layers are drawn using the same "technology", instead of some of them working differently.So maybe don't use "planes", just four identical layers - less confusion for you!

author: Psi
author_rank: Super Contributor
timestamp: November 23, 2017, 05:17:30 am
content: Using 'plane' layers is restrictive.I recommend 4 signal layers and make your power planes on the middle 2 signal layers yourself manually using pours

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 23, 2017, 06:41:58 am
content: Quote from: Siwastaja on November 22, 2017, 07:35:45 pmYes, I did it. I have set 4 layer signal instead of (2 signal later+2 planes).now my problem is:I have some sensitive nets as follow:I can pour polygon around it without any problem (consider with 20 mil clearance)also I should put ground layer under this layer. but this area should be ground free! this is my problem bcoz the sensitive nets are on the top layer!

author: Psi
author_rank: Super Contributor
timestamp: November 24, 2017, 11:05:54 am
content: Quote from: xzswq21 on November 23, 2017, 06:41:58 amsorry, what?Can you reword that.

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 24, 2017, 10:00:57 pm
content: the top layer has many nets and some of them are sensitive nets as you see above.the second layer is the ground layer. but under these sensitive nets should be ground free!3rd layer is the power layer.4th layer is the solder side.If I want to pour ground polygon in the second layer, this sensitive area will not be ground free! bcoz the nets are in the top layer and I'm in the second layer!

author: tautech
author_rank: Super Contributor
timestamp: November 24, 2017, 10:47:46 pm
content: Quote from: xzswq21 on November 24, 2017, 10:00:57 pmCould you just adjust the Keep Out border on the Gnd layer ?

author: Bud
author_rank: Super Contributor
timestamp: November 24, 2017, 11:35:39 pm
content: Quote from: xzswq21 on November 24, 2017, 10:00:57 pmYou have been told to use "polygon pour cutout" . What is the problem ? Learn how to use it.

author: mars01
author_rank: Contributor
timestamp: November 25, 2017, 09:56:44 pm
content: Quote from: xzswq21 on November 24, 2017, 10:00:57 pmHi,I believe that sometime some pictures may be of better help than a lot of words.Let's assume that you are using a 4 layer board.The layer stack is set as this:- TOP layer (signal layer)- GND layer (plane layer)- PWR layer (plane layer)- BOTTOM layer (signal layer)Signal layers are layers on which you lay traces and polygons and so on. Those are positive layers which means that wherever you see color (polygon pour, fill, traces etc) you will have copper on PCB.Plane layers are layers meant to serve as a connection for ground nets and power nets. Those layers are negative layers which means that whenever you place "something" (trace, polygon pour, fill etc) in that place occupied by that element, there will be a lack of copper on PCB.So, what you want is that under the region on top layer occupied by your marked components, on the GND plane, to have a void in the copper, a lack of copper.This can be obtained by placing a copper fill on the GNDplaneunder that TOP area. But the GND plane being a "plane" and therefore a negative layer, by placing a "copper fill" in the end you get a void in the copper.Please see the 2D view of such a board in the attached 2D.pngIn the 3D view of such a board found in the attached 3D.png, you can sort of see the copper void under the area with the "opamp".Attached is the Altium 18 PcbDoc file that I've setup and used to get those pictures.LE: I've added also a picture where I removed all the copper on the PWR plane (by placing a copper fill big as the board) and in the 3D view you can see that the copper is removed by placing that copper fill on GND plane.

author: xzswq21
author_rank: Frequent Contributor
timestamp: November 27, 2017, 06:04:39 pm
content: Quote from: mars01 on November 25, 2017, 09:56:44 pmDearyou placed a simple solid region under this sensitive area. what's the shape? is it a triangular?consider you have poured a ground polygon around this sensitive area at the top layer (with 20mil clearance)can you have a copy of this shape under this area? your solid region is not a copy of the polygon around this area at the top layer.

author: mars01
author_rank: Contributor
timestamp: November 27, 2017, 10:59:09 pm
content: Now, that your layer stack is made out of 4 signal layers, you can actually draw a polygon pour on your GND layer (the signal layer that you dedicated as GND).If you want the copper to stay out of that protected area (under your sensitive components) then you simply draw a keep-out solid region on that layer (your GND designated layer) and in Properties you selectRestricted for layer: Keep-out layer.You make sure that this Keep-Out solid region follow closely the perimeter of the protected area. Drawing is done manually.In Altium Designer 18 you press keys P -> K -> R with your GND designated layer as the active layer.