RF 50 Ohms Dummy Load PCB Design (High Frequency Ground Plane)

[OnurCan]

Hi I am a rookie on both RF and PCB design and I am currently trying to do a 50 Ohm 11 Watts Dummy Load project for 100MHz-1GHz. My calculations are done for the load but I have some questions about designing the PCB.

I am trying to do it as a microstrip line and as a simple structure of the circuit with only one signal I decided to do my design as a two layer PCB. Is it correct or enough?

I am trying to design so that the signal reaches all resistors at the same time because I want a high impedance with reflections and this is really difficult with so many resistors.

I need a ground plane for my design, I poured grounded copper only to the bottom layer and connect my Smd resistors with vias. Is this good enough or should I add an inner ground plane? I am having a hard time deciding how to do this ground plane. I will appeciate all suggestions for how to place a ground plane in this situation.

Project Specification: The power I am trying to terminate is 5-10 watts. Smd resistors are 560ohms 1 watt resistors and the signal strenght should not exceed -10dBm that is why I am using an 50dB attenuator, to achieve the desired signal strenght.
Here is what they want me to do exactly : ''Design and build a dummy load with 50 ohm impedance for the interval of 100-1000 MHz. The load shall have a power rating of at least 5 W in continuous mode, and have a measurement connector to connect to instruments. The signal strength in this connector should not exceed -10 dBm. ''

Top part of the circuit is attenuator written as AT1,AT2,AT3 Other resistors are for the load.

Pcb design Spesification: Trace Width = 0.5mm , Dielectric Thickness = 0.3mm , Trace Thickness = 0.036mm , Substrate Dielectric (Ɛr) = 4.6 Total board thickness = 0.39mm Size of the resistors (x,y) = (6.4,3.2)mm Dimensions of the board are (x,y) = (7.5,10)cm

I am using Altium Designer for this project. Thank you for your time

 

[JimB]

We have been in and out of this rabbit hole already:

50Ohm 11W Dummy Load with an attenuator.

Hey guys, I am doing a dummy load project for my Radio Frequency lecture and I am going to need help for this project. I first started with 11 parallel resistors design, each resistor is 560 ohms and 1 watt. There is a must in this project and that is the signal strenght should not exceed -10...

www.electro-tech-online.com

With that in mind why are you trying to do 50dB attenuation at 1Ghz in one step?

Your circuit board layout of the attenuator part appears to be wrong.
What sort of connector are you using for connection to "test equipment"?

Your circuit board layout for the dummy load is to say the least strange.
Consider something like this:

I have drawn this with vias as per your original drawing.
If I was building this I would have a groundplane on the top surface as well as the bottom surface and put vias where shown above.
Make the line which connects all the resistors to the input connector have a characteristic impedance of 50 Ohm.

JimB

 

[OnurCan]

Thank you for quick respond.
In the previous subject as you mentioned I explained seperated 20-20-10 ohms attenuator in the theoretical part of my project report and my instructor accepted it. I am doing this one step attenuator because it is easier to design and I am aware that it is not the best way of doing it thank you

I am using this https://www.snapeda.com/parts/0039296028/Molex/view-part/?ref=search&t=0039296028 , 2 pin connector header but I am open for your advice.

Do you think my two layered pcb with given thickness values are okay for a good 50 ohms impedence?

My concern is with having a grounded copper pour on the top layer is that having a controlled impedence will be pretty hard, what do you think?

 

[kubeek]

I would put the resistors in a circle around the connector.

 

[OnurCan]

Hi again, I did my design as your instructions like in the picture below. Everything is okay with the layers, ground, impedance and such.

I also tried to do it as a circle but I couldn't get out of this situation. My instructor keep saying that :
''There is a problem with lining up resistors on a row, because you will see a high impedance with reflections on first resistor, then traveling to the next, and the next ... Try designing so that the signal reaches all resistors at the same time. This is difficult with so many resistors. If the attenuator is then directly connected to the same point your series resistor can be of high impedance without affecting signal, because of the short length. ''

I am out of ideas and about to get crazy this is literally my 10th time re-sending this project please help me. Please keep in mind I didn't have any prior knowledge before starting this project and I am trying to learn.

 

[kubeek]

I don´t see why you couldn´t do a circle. Twelve resistors evenly spaced will give you three thin wires going in between each two ground pins, should be very easy to do. Or you could go thicker in four ways and than split each to three wires.
From one of those connections you can take the attenuator tap and be done with it.

Also, your connectors should have all the ground pins connected to gnd, not just one or two.

 

[OnurCan]

Or you could go thicker in four ways and than split each to three wires.

You mean something like this works?
And how can i decide the width of the thicker lines?

 

[kubeek]

Why dont you make it nice and symmetrical? something like this, offcourse all the lines shoud be equal and the parts should have more precise placement, the point where it divides into three as close to the center as possible, and the line from that point to the center pin should be about three times the width of the line going to the terminator. This is what I sketched in easyeda in about five minutes.

 

[kubeek]

Also, what is the impedance of your traces? It shoud be 600 ohms to match each terminating resistor, that likely means a thick pcb and a tiny trace width.

 

[OnurCan]

Trace thickness : 0.036mm
Substrate height : 0.3mm
Trace Width : 0.55mm
Substrate Dielectric : 4.3

When i calculate for these values it gives me 50 ohm impedance.
I didn't get why it should be 600 ohms?

 

[kubeek]

50 ohms should be at the center pin of the RF connector. But since each resistor is 600 ohms, to get 50 ohms termination when there are 12 in parallel, then the trace going to it should also have impedance close of 600 ohms. However even with 2.5mm substrate and 5mil trace the impedance is still only about 165ohms.
I am not really sure how smooth the transition from 50 ohms in the middle to twelve 600 ohm traces would be, but I think it should be much better than twelve 50 ohm traces.
But still, at 1Ghz the traces are really small compared to the wavelength so I don´t think there should be a big issue.

Will you be testing the final design on a vector analysator? If so, please post then the final design and the measured results.

 

[JimB]

On the one hand we have this startement:

In the previous subject as you mentioned I explained seperated 20-20-10 ohms attenuator in the theoretical part of my project report and my instructor accepted it. I am doing this one step attenuator because it is easier to design and I am aware that it is not the best way of doing it thank you

Stating that you are using an attenuator which will not have the design attenuation values above some relatively low frequency.

And on the other hand we have

''There is a problem with lining up resistors on a row, because you will see a high impedance with reflections on first resistor, then traveling to the next, and the next ... Try designing so that the signal reaches all resistors at the same time.

All without building an test jig to try and evaluate the design.

Also consider that all this mental ache is brought about by using a handful of 560 Ohm resistors, rather than one correctly sized 50 Ohm resistor.

If you are so worried about the impedance of the line from the RF connector to the resistors, you could always try a line with a stepped width, so that the impedance rises in step, changing at each resistor pair to represent the load at that point on the line.
Or in a similar way, you could try a tapered line.

By the way, what is that connector after the attenuator that you are using for connection to the test equipment?

JimB

 

[OnurCan]

Hi I am writing this as a feedback so my design overall with so many 560ohm resistor is not an optional design as you say. Therefore I decided to do it with less resistors with higher power. Because routing the 12 parallel resistors with 600ohm impedance is really hard and not optional.

I think it is better to go with two parallel 100ohms, 5 watt resistors. I will re-design the pcb.

Knowing we are not alone and someone out there actually care for your problem is such a good feeling. Thank you all for your help.

 

[Nigel Goodwin]

Hi I am writing this as a feedback so my design overall with so many 560ohm resistor is not an optional design as you say. Therefore I decided to do it with less resistors with higher power. Because routing the 12 parallel resistors with 600ohm impedance is really hard and not optional.

I think it is better to go with two parallel 100ohms, 5 watt resistors. I will re-design the pcb.

Where are you going to find 5W non-inductive resistors?.

The whole issue with dummy loads is making them purely resistive, and not inductive.

 

[OnurCan]

Where are you going to find 5W non-inductive resistors?.

The whole issue with dummy loads is making them purely resistive, and not inductive.

I thought using two of this would work https://www.digikey.com/product-det...ssive-product/3550100RJT/A143824CT-ND/9928279
What do you think about this resistor? Would it work or should I go for a design with more resistors with lower power rate?

 

[Nigel Goodwin]

Hard to say, as there's no mention of inductance in the datasheet.

 

[rjenkinsgb]

Why the complication of a PCB?

You can make a very effective multi-resistor dummy load "squirrel cage" style, a with copper or brass ring or just solder tags on the connector body and the resistors all arranged parallel to the axis, soldered to the earth ring at one end and the other end leads bent inwards to the centre pin; or use another disc on that for connection.

This is a small one with just two resistors, but is shows the concept. I have one somewhere I built many years ago with eleven, 560R 2W carbon resistors spaced around an N type socket.

http://aeroelectric.com/Pictures/Tools/RF_Antenna_Test_Tools/DummyLoad.jpg

As long as the connections are kept reasonably short, they are fine to well over 1GHz.

 

[Nigel Goodwin]

Why the complication of a PCB?

Because it's a school/college assignment, not an actual project.

 

[OnurCan]

Why the complication of a PCB?

You can make a very effective multi-resistor dummy load "squirrel cage" style, a with copper or brass ring or just solder tags on the connector body and the resistors all arranged parallel to the axis, soldered to the earth ring at one end and the other end leads bent inwards to the centre pin; or use another disc on that for connection.

Yes I agree with you. Actually I pick this subject because I thought I was going to do it as you say without the PCB. But my instructor wants it this way.

I will update my progress here In the mean time I am open to suggestions if you have any since I am doing it from the beginning.
Thank you for your time

 

[JimB]

Why the complication of a PCB?

This is one of those college/university projects which seem to be heavy on theory, and light on hard practical experience.

It would be good if OnurCan could just knock up a circuit board and test it in the lab to see how good/bad it is and learn form the experience.
But I think that the virus thing means that he is working from home in a bit of a vacuum.

I think it is better to go with two parallel 100ohms, 5 watt resistors. I will re-design the pcb.

Yes that would be better I think. But don't forget the effects of adding the attenuator.


JimB