a doubt about Ground coplanar waveguide VS microstrip

microstrip vs coplanar waveguide

Most of the papers say that the ground coplanar waveguide's performance will better than microstrip. but When I simulated with ADS to

find the difference between then, I found that the coplanar waveguide's performance is not better than microstrip.
is my simulation setting config wrong?
is my simulation method wrong?

wish you can give me some good ideas about it.

thanks in advanced.

grounded coplanar waveguide (cpwg)

I checked your simulations and got similar results (see included files). Actual loss in transmission lines comprised from two major factors: conductor loss and dielectric loss. The first depends on trace geometry and material whereas the second depends on dielectric properties and geometry. Both relay on frequency. The first picture shows simulation for the case without ground plane under CPW and the second done with ground plane. As you can see from the pictures CPW with ground plane has less insertion loss and better return loss. Both simulation were done simultaneously with LINC2 RF simulator (it is easier and faster than ADS). All TLs and substrates parameters are the same as shown on your picture.
However, if you look carefully on results, you note than CPW results are pretty good and in practice (with real PCB and all manufacturing tolerances accounted) the difference is negligible. From another hand CPW has better isolation on the board and less coupled to other circuits. It also provides more freedom for trace width and board thickness.

how to em silmulation of cpwg line

Regarding this subject I know that opinions are divided. Now depends by application.
Myself I am not a big fan of CPW even the performances suppose to be better than microstrip. Possibility to fail in high volume production is higher when using CPW (due to multiple factors). In general I am using CPW only in reference designs and prototypes.

waveguide to microstrip

Yes, it is not easy question and a lot depend on application and design. CPW allows much more freedom in design and often designer may do CPW less depended on manufacturing process than MS. I have good experience with CPW and it is preferable TL for me because my job is UWB design. For very broadband system CPW have better isolation and flexibility. It is a bit harder to calculate because it required solutions for elliptic integrals of the first and second kind, but once prepared worksheet can do the job. I included all analyzes for manufacturing accuracy sensitivity and dielectric constant variation. What is necessary is just to insert a few numbers and you immediately get all the information and can play with these numbers to find the best solution. Usually it takes only a few minutes. So design practically is not more complex than for MS.

calculating gcpw trace width

Here is not about hard or easy to design a simple transmission line. I am talking about behavior on high volume production, more than a million boards per month (e.g. mobile phones).
UWB products will need a few years from now to arrive to this volume…or maybe never.

grounded coplanar waveguide fr4

Are you using CPW or CPWG for UWB? CPWG has a MS mode and CPW mode so the dispersion is worse than either MS or CPW.

I have found that CPWG gives a little more isolation but it's not great; maybe 6 dB for lines spaced a a few substrate thickness apart. I just use plain MS and space a ground about one substrate thickness away. That helps a little with isolation but is not coupled enough to be CPWG.

coplanar waveguide with ground

thanks all of your good idea, and I have another question

In ads which the H means?? it means the microstrip to reference GND?? or it means the all thick of the board?? please see the attachment Picture.

and I also made another calculate on CPWG and MS, just the microstrip to refer gnd is 25.2mils the microstrip will 47mil

In CPWG I found that if I choose the width is 47mils and the gap is also 47mils , the impedance is just 50 ohm

rf design linc2 opinions forum

i found that the Gap equals to the CPWG line width is near 50 ohm than the
Gap equals to 2X CPWG line width
But usually we will keep 2times distance to the signal line for coupling problem


does any body can give some idea on the distance to the nearby Ground problem for coupling. (not the distance to the reference gnd)

microstrip vs cpw

To vfone,
I agree with importance of high volume production and this is why I told about importance of having precise, fast and easy to use tool to design CPW. For example, when I was a member of cell phone design team in one of Motorola design centers about 10 years ago, we try to use CPW. For these times we had only one tool and this tool was bulky and not accurate, so we drop CPW. Then in another company I met the same problem with CPW. After this I spent significant amount of time to study the problem and design the worksheet. Now we do CPW design quickly and easy and have no manufacturing problems. I use it not only for UWB due to consulting other companies. By the way, UWB products may reach several millions volume before the end of the year. We have a products and market needs them.

To madengr,
I use both of them. The choice depends on particular application and even on the same board may be different situation. May major point is to play with design variables and get result which provides stable manufacturing and required RF performance. I can easily do isolation up to 90 dB. Higher numbers are possible, but may be not stable and will require additional measures. If you have 6 dB isolation with CPW something is definitely wrong. I am going to publish technical paper about isolation optimization for PCB layout and there will be detailed recommendations on CPW too.

coplanar waveguide reference ground

If you have 6 dB isolation with CPW something is definitely wrong. I am going to publish technical paper about isolation optimization for PCB layout and there will be detailed recommendations on CPW too.

Click to expand...

Actually about 6 dB more isolation than plain microstrip (spaced a few substrate thicknesses). I look froward to reading your paper. Please let us know when it is complete.

microstrip coplaner waveguide

To bless_fooling,
1. For both CPW and MS H value means the shortest length of field lines, or distance from trace to lower ground. Board thickness is different.
2. In CPW trace width depends on Er, substrate height and gap whereas for MS it depends on Er and substrate height, so you have more freedom in these parameters combination for CPW. These two TLs have different field distribution and it also depends on TL geometry and dimensions. You may change MS trace width and make it desirable value by choosing different substrate height if it is possible. In CPW you may change the trace width even for fixed substrate height by changing gap. You also may change the effect from lower ground plane in CPW. Let’s see one simple example when we have CPW on FR4 substrate with Er=4.5 and H=0.508 mm, copper is 0.5 oz (0.0174 mm). In this case 0.74 mm wide trace and 0.3 mm wide gap provide Zo=50.14 Ohm. The distance to lower ground is about 70% bigger than to upper ground. Now we want to reduce the effect from lower ground and decrease gap twice to 0.15 mm. Trace width goes down to 0.525 mm and we have about 249% difference between ground distances and the same Zo. We decrease effect from lower ground and manufacturing uncertainties from substrate height variations but increase it for gap variations.
3. You are right. When gap become too wide CPW become more MS than CPW. The best way to check all this stuff is to use Polar filed solver or EM simulation. At first design your CPW and then check it with Polar or another EM simulator. To illustrate dependents of CPW Zo on design variables I included two pictures for FR4 0.508mm substrate. Please check them. These results were obtained with MathCAD based worksheet and consider more parameters than we discussed (like board coating and so on).

coplanar waveguide pcb

thanks all of your good idea, I benefit a lot.
Now i know a little how to deal with MS or CPWG

cpwg microstrip mode

I have been watching this thread with some interest.

Just another couple of comments:

CPW and GCPW lines have another convenient feature, namely, if you want to add shunt components it is relatively easy compared to a ms line where the groundplane is on the other side of the board and not so accessable.

I have not seen a discussion of how via's play into this mix (GCPW). This opens the question about when is a field solver needed vs Polar or some other tool.

when does microstrip become coplaner

It is very interesting area of via usage and optimization, their effect on CPW and parasitic oscillations inside the board. But initial question did not touched this area and it is more suitable for separate discussion. Regarding tools I think that well prepared worksheets are the best for initial design and than you will do EM simulation for all RF part of the board any way and it show what is going on between via. I believe that applying EM simulation to small part of the board (e.g. to CPW alone) will not provide the whole picture and design probably will not be the first pass.

coplanar waveguide design pcb

Dose you simulation the CPWG (include with vias ) with CST or Other tools??
can you kindly recommend it??

thanks in advanced.

coplanar waveguide with lower ground plane

The plots what I posted for you were obtained with numerical calculations with MathCAD worksheet and with suggestion of good ground. They do not include any EM simulation. This is first round of CPW design. Then you make ground good (e.g. with via) and include CPW into board design. Now it can be EM simulated in whole for final checking. Please read posts above again if you missed something.

microstrip to cpw

Dear RF-OM,
Could you share the Mathcad worksheet for me.
I have been searching for CPW equations for some time.