Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Microstrip vs. Grounded co-planar

Status
Not open for further replies.

Jim cage

Full Member level 3
Joined
Jul 2, 2006
Messages
150
Helped
13
Reputation
26
Reaction score
7
Trophy points
1,298
Activity points
2,163
Hi,

Can anyone tell me what is the difference between Microstrip and Grounded co-planar?

If you take a grounded co-planar waveguide and separate the two ground conductors (near the center trace) to infinity, why wont you get a microstrip line?

as I understand, microstrip is a trace where the ground is located below the trace.
Coplanar has a center conductor, 2 ground trace distanced at a GAP and a ground plane below.

Regards,
Jim
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
The coplanar with ground plane is slightly better than ordinary microstrip. The main advantage is that you can have shunt elements to ground without the parasitics of vias. This is very important when you get into the 4+ GHz region. The US company Hittite always has coplanar with ground in their suggested layout application notes.
 

Jim cage

Full Member level 3
Joined
Jul 2, 2006
Messages
150
Helped
13
Reputation
26
Reaction score
7
Trophy points
1,298
Activity points
2,163
1. But why when you enter a gap distance of infinity you are not getting the characteristic impedance of a microstrip?

(use ADS(Linecalc), TXLine or Appcad and you will see that if you take co-planar with a ground plane and have a gap distance of 1000000mil for example between the center conductor and the other two you are not getting the characteristic impedance of a microstrip)


2. Another questions, when you manufactor a PCB there is always a stage where they fill out the entire CS with ground on the empty spots. this means that the microstrip is now turning to co-planar right? (near each conductor there is ground now...)


Regards,
 

Azulykit

Advanced Member level 4
Joined
Feb 18, 2007
Messages
1,121
Helped
219
Reputation
436
Reaction score
112
Trophy points
1,343
Location
All over the Map.
Activity points
8,407
There are two very useful books on various PCB transmission line forms. Simon and Waddel (I have paper copies). You might want to run them down.

Your descriptions are correct. MICROSTRIP is a thin trace over a larger (often much larger groundplane). COPLANAR WAVEGUIDE is a trace with groundplanes (or sidegrounds) on both sides and all in the same plane. GROUNDED CPW is similar, with a trace and sidegrounds (groundplanes) ....and....a groundplane under the trace and sidegrounds. Usually the sidegrounds and lower groundplane are connected with "stitching" vias. This is what makes the convenient connections that Flatulent describes.

If the gaps are increased significantly, grounded CPW will (generallly) have the same impedance as microstrip.

Just a warning, the thickness and dielectric constant play into this in a big way and one often sees unexpected impedance trends when just the gap is changed. I guess one could think of flooding the area around a trace as converting microstrip to grounded CPW. I would expect to see the addition of vias as well if that is the objective.
 

RF-OM

Advanced Member level 2
Joined
Aug 3, 2007
Messages
584
Helped
123
Reputation
246
Reaction score
17
Trophy points
1,298
Location
The Earth
Activity points
5,751
The major difference between microstrip and coplanar structures is in modes. Coplanar is better when it is real coplanar (when slot is narrower than substrate height). The reason of wrong results when you try to use AppCAD or similar program is in the quality of these programs. Simple programs usually use kind of simple numerical algorithms for calculations. Such algorithms are based on some assumptions, first of all on ratio of trace width to substrate height as well is for slot width. Such empirical approach works well only when ratios are within the suggested limits which definitely are not very wide. Many numerical approaches use simplified solution for elliptic integrals of the first and second kind. This works well for many practical scenarios, but not for very high slot width. If you want to check coplanar with very wide slot you need to use one of field solver simulators.

Best regards
 

ADS_RFMW

Full Member level 2
Joined
Aug 18, 2005
Messages
126
Helped
7
Reputation
14
Reaction score
4
Trophy points
1,298
Activity points
1,797
Use Agilent Momentum that gives you exact expected results
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
One thing to watch out for in free or low cost transmission line programs is putting in dimensions outside the range of validity of the algebraic equations these programs use.

The advice above about using a field solver program is wise. These programs are more expensive but are more exact for any set of dimensions.
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top