[ADS] generating layout from schematics

[volker@muehlhaus]

im using microstrip and not coplanar. what im looking for is ground separation between micro strip runners.

Understood, and GCPW would be a possible way to create these side ground strips.

But you can also draw them by hand in layout: rectangle or polygon on layer "cond" for metal, circle for vias on your via layer. Not sure what you via layer is - typically it is "hole" but you can check in layout.

how if i need accurate electrical model from schematic?

???

 

[pragash]

1) please refer to figure below. i have two vias to ground in schematic but when i click "generate/update layout" in translate to one via in layout which is wrong. how can i generate two vias in layout?



2) does ADS have any layout component for DC supply? please refer to figure below.



3) the whole point of me doing layout in ADS is to correct the layout if in case its affecting the circuit performance. after generating the layout, how can simulate the layout? Am i need to simulate the layout in EMDS/momentum and then create schematic component and simulate that in schematic by connecting lumped element? any short cut way? im using ads2015.

4) how to release gerber in ADS?

- - - Updated - - -

5)

If you want to EM-simulate it and don't need an accurate electrical model from schematic, you can define another MSUB and map other layers in that MSUB. Than all elements using that second MSUB will draw on the layers defined there.

actually i need accurate electrical model from schematic. the whole point of me doing layout in ADS is to correct the layout if in case its affecting the circuit performance. how can generate multilayer PCB in this case. i need to generate 8 layer board. how can use MSUB to do it? In ADS cond and cond2 are default conductor layers. what are the 3rd, 4th, 5th, 6th, 7th and 8th conductor layer i can define using MSUB? how to define my 7 dielectric layer? i need to choose the name of the layer from ADS layer list as below? please elaborate since im confused in this area:-( please refer to pic below for layer list in ADS!




6) Ads have 255 layers!!! this so many layers confusing me! is it means whatever layer i define in MSUB only will be used? all other layers will be neglected?

 

[volker@muehlhaus]

1) please refer to figure below. i have two vias to ground in schematic but when i click "generate/update layout" in translate to one via in layout which is wrong. how can i generate two vias in layout?

You have placed two vias in parallel in schematic, and you get two vias at the same position in layout. Just move them as needed.

2) does ADS have any layout component for DC supply? please refer to figure below.

It is easiest to draw a pad yourself.

3) the whole point of me doing layout in ADS is to correct the layout if in case its affecting the circuit performance. after generating the layout, how can simulate the layout? Am i need to simulate the layout in EMDS/momentum and then create schematic component and simulate that in schematic by connecting lumped element? any short cut way? im using ads2015.

Yes, you can use results from EM for the layout for the parts that have no schematic model (easy) or for the full layout (requires more EM experience). This is your engineering decision.

4) how to release gerber in ADS?

In layout, export artwork in File menu.

how can generate multilayer PCB in this case. i need to generate 8 layer board.

The microstrip parts that you have shown are on the "outer" layers? And you will take it into a "real" PCB" layout program to combine it with digital circuit that needs 8 layers?

how can use MSUB to do it? In ADS cond and cond2 are default conductor layers. what are the 3rd, 4th, 5th, 6th, 7th and 8th conductor layer i can define using MSUB?

Micorstrip is for one conductor layer over a ground plane. In a multilayer, these are the "outside" layers on top and/or bottom. The inner layers are usually not drawn in ADS.

how to define my 7 dielectric layer? i need to choose the name of the layer from ADS layer list as below? please elaborate since im confused in this area

I would use Momentum and run things in Momentum if there is coupling between layers and multiple dielectrics needed. But for microstrip we typically have that ground plane that shields the top conductor from everything below the ground plane. Then you can simulate them separately.

6) Ads have 255 layers!!! this so many layers confusing me! is it means whatever layer i define in MSUB only will be used? all other layers will be neglected?

Even if you have 8 metal layers, every layout system has more than 8 drawing layers. There are extra layers for solder mask, component print and other functions. So the number of layout layers is larger than the number of conductor layers.

In ADS, the predefined layers also include layer names for 8-layer PCB: pc1, pc2, pc3, ... and pcvia1, pcvia2, ...
This is because ADS designers want to give you a choice what layer names you want to use. But these are only names, and there is no difference in functionality. You can use "cond" or "pc1" and the difference is only the name. You can use (almost) any layer name - just map it to the correct physical position if you are using Momentum.

Now that you have an idea how to start, it is a good time for a Keysight ADS training. These are really good to learn more about the tool and workflow.

 

[pragash]

The microstrip parts that you have shown are on the "outer" layers?

yes.

And you will take it into a "real" PCB" layout program to combine it with digital circuit that needs 8 layers?

no. im planning to do complete layout in ADS and release gerber in ADS.

- - - Updated - - -

the digital are in inner layer..

- - - Updated - - -

Micorstrip is for one conductor layer over a ground plane. In a multilayer, these are the "outside" layers on top and/or bottom. The inner layers are usually not drawn in ADS.

ok. so the ADS gerber will be generated only for top and bottom layer. i have to tell the fabrication company about how i want inner layers to be so they will do accordingly?

- - - Updated - - -

I would use Momentum and run things in Momentum if there is coupling between layers and multiple dielectrics needed.

are you talking about defining in EMDS window as shown in above pic and run Em simulation?

But for microstrip we typically have that ground plane that shields the top conductor from everything below the ground plane. Then you can simulate them separately.

understood. my DC is coming from bottom layer to top layer. my top layer has RF section. i can neglect long DC trace from bottom and connect the DC source directly at the top. please explain what you mean by "Then you can simulate them separately".

- - - Updated - - -

You have placed two vias in parallel in schematic, and you get two vias at the same position in layout. Just move them as needed.

is there any schematic component to place adjacent vias in layout?


thanks alot for the help so far. your inputs really helping me to generate layout. i appreciate that

 

[volker@muehlhaus]

no. im planning to do complete layout in ADS and release gerber in ADS.

Ok, then you will need to do "manual" routing in ADS layout. That is certainly possible.

ok. so the ADS gerber will be generated only for top and bottom layer. i have to tell the fabrication company about how i want inner layers to be so they will do accordingly?

No, that is misunderstanding!

You can draw in ADS layout on 2, 8 or 50 layers. As many as you need. And easily export that to Gerber.

are you talking about defining in EMDS window as shown in above pic and run Em simulation?

Yes, I was talking about the substrate definition used in this emSetup. But why EMDS? It is much easier to use Momentum for this PCB work.

understood. my DC is coming from bottom layer to top layer. my top layer has RF section. i can neglect long DC trace from bottom and connect the DC source directly at the top. please explain what you mean by "Then you can simulate them separately".

Do EM simulation with multiple small EM blocks instead of one big EM block - if you know that EM coupling between the parts is small.

is there any schematic component to place adjacent vias in layout?

No, only if you place the two vias at a distance with all the small MLIN/MTEE. But you can also define a subcircuit for two vias, and use that in your design. Start learning manual layout in ADS (not auto-generated from schematic), you will often need that in the future.

Good luck!

 

[pragash]

No, only if you place the two vias at a distance with all the small MLIN/MTEE. But you can also define a subcircuit for two vias, and use that in your design. Start learning manual layout in ADS (not auto-generated from schematic), you will often need that in the future

great idea! thanks.

Ok, then you will need to do "manual" routing in ADS layout. That is certainly possible.

based on your input and my exercise, i know that all the lumped element pads, routings (trace) and vias (even multiple vias) can be generated using "generate/update layout". the only manual work i need to do is creating power supply pad, creating ground plane at top layer and also inner layers. please explain why i need to go back to zero and manually re-create the routing if i want to generate the gerber. why can i use existing generate/update layout routing, component pads and vias and just create planes (power and ground) to complete the design?

- - - Updated - - -

how can generate multilayer PCB in this case. i need to generate 8 layer board. the microstrip parts that i have shown are on the "outer" layers. i will just use ADS to generate my multilayer/8 layer PCB. please advice.

 

[volker@muehlhaus]

use existing generate/update layout routing, component pads and vias and just create planes (power and ground) to complete the design?

Yes, you just need to add the missing pieces. I was assuming that you have much more layout to do if you use 8 layers.

 

[pragash]

im designing an amplifier board. im thinking of using 3 layers, top for RF, bottom for DC and middle for ground plane. i said 8 layer for worse case example/future. thanks alot dr volker.