Where can i fabricate microstrip and help with GENESYS

[RF-OM]

Your filter is narrow band so there is not so much what you can do.

1.You can increase unloaded resonators Q. The major factors to consider are conductor loss and dielectric loss as well as matching. You can model them numerically which is the best method or try to use simulators. Genesys usually gave me results that were very close to bench test. If you will use Rogers material you may get good results.

2. Next check how much do you lose on connectors. Very often there is about a half of loses. Especially important is to have right footprint and metal go to the very end of the board in connector area. The signal trace must go to the end of the board and central pin must be soldered along all the length.

3. The last point is to try to tune filter into Genesys. Filters are designed by special mathematical algorithms. But not all of them were discovered and you may empirically find better solution. It is possible, I did it many times. It is tedious work, but if you are patient and know filters well you may get much better filter that designed by known algorithm.

By the way, check your filter one more time. It is not well tuned or matched. The left part of pass band in skewed. Otherwise it looks good.

 

[selva500]

Thanks for the advice. So is the -4dB loss reasonable. In other words, from your experience is this type value of loss expected in a microstrip design (what is the usual range?) or is mine not a good design?

My designs are fabricated on the Rogers material that I obtained. The connector losses could be a factor. There is a small gap between the edge of the board and the signal trace on my PCB. I could possibly reduce this as you said.

As for tuning, how do you go about doing this efficiently in GENESYS? Do you have any tips for that? I tried doing a monte carlo analysis and playing around with the number's obtained frm that analysis but the automatic optimisation seems to give the best response in the EM simulation at least. When tuning is it better to look at the EM response or the linear response. The linear response seems to be more sensitive to the tuning in my case at least.

I'm not sure why the passband is a bit skewed. I made sure all the lines and input/output cables and equipment have 50ohm impedance. Could there be any other reason for this? I was only able to look at the amplitude response using a spectrum analyser as I dont have access to a network analyser at the moment but my university is purchasing one and it should arrive next week sometime. That could possibly give me a better idea of what is going on. Out of my 3 designs, the edgecoupled one has the most symettrical looking passband but unfortunately the center frequency is off by some margin. Also the size of it makes it unappealing.

Thanks for your time again. If anyone else has any inputs I would appreciate it.

 

[RF-OM]

Insertion loss -4dB is reasonable for such a narrow filter. But you may try to make it better as I describe earlier. There is no guarantee but why not to try? If you have a gap in trace-to-connector pin connections it means you have a piece of wire (central pin) that hanging in the air. There is about 1nH per 1 mm inductance or about 6.3 Ohm per 1 GHz of frequency. With your 2.2GHz frequency it means about 14 Ohm per 1 mm of unsoldered to the trace pin. If you have TDR it is easy to see what is going on with this connection. My experience show that 0.25mm of gap in ground plane and board edge plus about 0.5-to-1mm gap into connector’s pin will give about 6 dB of power loss (!) at 4GHz. So, this may be very serious problem.

I usually do all design with schematic simulation but shift all frequencies up for about 10%. When I tuned everything I verify design with EM simulation (it is pretty long) and it shows response close to the right one. This is usually enough to get good match with bench test (about 1.5-to-5% accuracy). But it is for well known material and filter type. If you do new design it is probably will require a couple of protos to find good correction coefficient for initial design.

Definitely Monte Carlo analysis has nothing common with tuning. This analysis can only show some expectation of yield. Try to do optimization first and stop it when you do not see any improvement for some time. Then do fine tuning manually. With some skills it is not hard even for 11th order filters. Chose small tuning increment and then go step by step.

Next time when you order the boards include small coupons. One may be for checking trace impedance to be sure that fab did a good job. Another may be short line with two connectors at the edges to check connector related insertion loss. You can even make your own calibration standards for network analyzer and de-embedd connectors together with the board and get pure filter’s S-parameters file. This is the best because it allows you to use this file later for simulations.

Do not be frustrated with small problems. Filter design is very complicated work and require long learning curve. But when you teach yourself to do it you can design excellent filters quick and with good match between design and actual measurements.

I hope it help.

 

[selva500]

Hello again,

I'm at the stage where i want to integrate my filter together with an LNA. This is going to be used at the receiver end of a ground station for a student satellite project. The LNA+filter will be connected to the satellite dish and it is meant to filter a certain frequency range and amplify it for further processing. The LNA i will be using is shown in the data sheet below:
https://www.hittite.com/content/documents/data_sheet/hmc548lp3.pdf

As it can be seen there are two stages of amplification. The filter is meant to be connected between the two stages. My question is would the presence of the LNA and its associated components/tracks will affect the performance of the filter at all since it is a microstrip design. Is there a way to migitate the effects? They have shown an evaluation board with a filter attached to the LNA but i doubt it is a microstrip based filter. Would anyone be able to advise on this?

Also i will need to design the PCB for the LNA using Alt1um Pr0tel. The issue is that my filter design was generated in GENESYS. Is there a way I can import the filter design from Genesys to Pr0tel. Can i export it as a gerber file and then import it into Protel or is there some other way to go about this?

Thanks for your time. Any inputs will be much appreciated.

 

[RF-OM]

You need to keep transmission lines as short as it possible because they are multiplying reactance. Your filter is relatively narrow, so matching may correct the lines effect. Hittite LNA has the S-parameter file, so you may simulate your filter with LNA and models for lines. It is not difficult task, then if it necessary design matching circuit. Transmission lines may be microstrip or CPW. Both will work well, CPW may provide better isolation.
On evaluation board chip size ceramic filter is shown with CPW, which is better in this case due to small distance between input and output of the filter.
Genesys allow you to export Gerber file and it is the best way. Remember that layout window must be activated in order to export Gerber file.
Good luck with your project.

 

[selva500]

Thanks for your input as usual. When u say matching, do you mean all the signal lines should be 50ohms. This is already the case in my filter and the LNA specs say the same thing as well. In terms of keeping the transmission lines as short as possible, I'm in a bit of a fix as the LNA package is 3mm x 3mm and since im using my own filter design and not a commercial ceramic filter, you can imagine is much bigger, around 5cm(width) x 3cm(height) which means that the final PCB will have to accomodate for the size of the filter leading which may lead to the transmission lines from the LNA to filter and vice versa being longer.

Also u mentioned using the LNA S-parameter file that i can use to simulate the LNA and filter. I'm not sure how to go about doing this or what software i need to use for this purpose.How do i use the S-parameter file to simulate the LNA?

As my filter is a microstrip based one, would designing the circuit using CPW affect it in any way? According to a website i visited regarding CPW (**broken link removed**). It stated that:
As mentioned preciously, if you want to make compact circuits using narrow transmission lines, you must trade off RF loss. CPW circuits can be lossier than comparable microstrip circuits, if you need a compact layout.

In terms of circuit size, CPW is at a disadvantage versus a stripline of microstrip circuit, because it's effective dielectric constant is lower (half of the fields are in air).

Does this mean that I have to modify my filter design (size etc) if i choose to go with a CPW based design or can the microstrip and CPW design coexist together on the same board? Would i be ok if i just went for microstrip design for the whole board?

I'm sorry for the many questions and if i seem not very knowledgeable regarding this. Unfortunately the lecturers in my university are not very experienced in this field either so it's left to me to try and get as much info and do things right.

 

[RF-OM]

When Transmission Line (TL) has 50 Ohm characteristic impedance pure 50 Ohm will be seen on one end only when the second is terminated by purely resistive 50 Ohm. This practically impossible in real life and your TL is always loaded with some reactance. In this case TL will multiply this reactance (rotate it around Smith Chart clockwise). This means that when you connect your LNA to the filter through TL filter will not see purely resistive 50 Ohm load and there probably need matching circuit. The same for the second side connection from filter to the next LNA.

Your filter looks to be only about 5 mm wide (if I remember right). You do not need to count feeding lines. Just connect LNAs with TLs to the feeding points of the edge resonators. Your filter only of the 3rd order, so there is no need for high isolation and microstrip should work well.

S-parameter file allows you to calculate actual impedance of the LNA. You can do it by yourself, just calculate Z=R+(or-)jX. If your file in RI format you already have the numbers and all you need to do it is just multiply them by 50 and you will get impedance. If your file in another format: MA or dB you need to transfer the numbers into simple numerical form RI. Simulation program will do it for you automatically and calculate the matching circuits if necessary. If you need all the equations to calculate impedance from S-parameter file and then determine what filter will see from another TL end, please let me know. I will try to find these formulas for you.

 

[selva500]

Hi again,

I see what you mean by the matching circuits now. I have had a look at the s-parameter file for the LNA and in it the manipulating variable is the frequency while the dependent ones are the s-parameters and something called YP, im unsure if this is the admittance, in which case it would be the inverse of the impedance. Would you be able to have a look at the file and confirm with me if the impedance is just the inverse of YP or is there something else i should be looking for. The file is available at: https://www.hittite.com/content/documents/sparam/HMC548LP3.zip

You said that the simulation program will be able to calculate the matching circuit, does Genesys do this? If so how do i acheive that?

I'm not sure how to relate the S-parameter file of the LNA and combine it while simulating the filter. I have managed to load the s-parameter file into the filter project but how do i set the simulation to take account for the these files? Do i have to create a component for the LNA and attach the s-parameter files to it somehow? After that would i connect the LNA and filter in the schematic so that it comes out connected in the layout? I'm sorry if the question is not so clear but I'm not sure how else to explain it.

I have actually changed the topology im using to a hairpin one as out of all the protoype filters i designed it had the best response. Hence the bigger size for it. I might try to redesign an interdigital one as well when i manufacture the boards with the LNA footprint on it as well. I have attached a picture of the design in currently using. Do you think the size, which is much larger than the LNA will affect the total performance? Also in this case you said there is no need for feed lines when connecting the LNA, does that mean i connect the TL straight from the LNA to the edge resonator (if there isnt a need for a matching circuit that is).

I hope you are able to understand my questions as i can imagine it would be difficult for someone reading this to comprehend fully what im trying to say. Thanks again.

 

[RF-OM]

I checked your S-parameter files, they are normal 2-port files without noise parameters. Format is MA which is Magnitude and Angle. You can use Genesys. Just find 2-port device (black box) and assign your S-parameters files for the 1st LNA to this device. Then use your filter design as it is or as a one more black box with filter’s S-parameters. Next insert one more black box with 2nd LNA S-parameters. Connect all these parts with transmission lines that you are going to use on your board along with actual substrate. Now you can simulate the whole system. If there will be big ripple it means your filter have poor matching. In this case you have two choices: use Genesys’ Match module or insert simple matching circuits into your schematic and match filter there. You even can use Genesys’ Optimization feature for this.
Hairpin filter is much bigger than interdigital, so TL will be longer. Unfortunately my office computer has problems when downloading files from EDAboard site and often do not open them. I cannot check your hairpin design.
In Genesys you can turn on layour feature and when you finalize your design you can simulate the whole system with Empower EM simulator. It usually provides good results if you do everything right.

 

[selva500]

Hi again,

I tried to simulate the filter along with the LNA S-parameter files using the way you suggested. When i do that though my filter's bandwith narrows dramatically. I'm not sure if this is due to matching or some other factor. I also tried implementing a matching circuit using the MATCH module but that gave me not so good results which makes me think that I'm doing something wrong. In the match module there is an option of specifying the input and output impedance to generate the matching circuit. Im not sure what values I should be putting in those as theoretically both the LNA output and filter input should be 50ohm which defeats the purpose of the matching circuit to begin with. I've only been looking at the linear response so far and not EMPower as even the linear response does not look good so I doubt there is any point in running an EM simulation at this stage. I have uploaded some of my workspaces online, it would be great if you could have a look at them and point out where I'm doing things wrong and suggest ways that i could overcome them. In the zip file, there are 3 workspaces.
Hairpin: is just the filter design by itself
Hairpin with LNA: filter and LNA simulated using 2-port black box
Hairpin with LNA & Matching: filter, LNA and matching circuit

You could download my zip file at:
**broken link removed**

Also when using a black box, does it matter if it appears on the layout window when running EMPower, as the black box does not have a footprint so I just used the 'Replace part with short' in the layout options of the blackbox. Thanks again. Hope to hear from you soon.

 

[RF-OM]

You made mistake in hairpin-with LNA worksheet. You need to assign S-parameter file to the block you chose. You chose dataset, but S-parameter file should be instead . Double click on LNA and go to Simulation tab there you may chose right S-parameter file. Do the same for the second LNA. After this you will be able to simulate your LNAs with filter. Based on filter plots there should not be any problems with matching. If you need to change footprint go to General tab and you will see line for footprint in lower part of the window. In very unlikely case if you need to do match you can add L-matching circuits and play with them. Datasets are not as good as S-parameter files because they have only magnitudes. Filter itself looks good but Monte Carlo shows strong dependents on component accuracy. You need to keep it in mind. Be raedy to see from EM simulation that filter is shifted down for about 10 to 20%. In this case you need to redesign the filter with shifting by the same shift up.

 

[selva500]

Hi,

I tried using the datafile instead of dataset option to upload the LNA S-parameter files but i still get the same response for my filter. The bandwidth of 100 MHz becomes really narrow so that it only focuses on the center frequency. I even tried uploading the file under the parameter option in the LNA part and still the response is similar. I'm wondering if you got a different response when u tried using the datafile option? Or is this a feature of the LNA that it focuses only towards the center frequency of the filter. Im not too sure about this.I have uploaded my latest workspace at:
**broken link removed**

Hopefully you can point out to me what is it that I have done wrong as I'm a bit confused now because all 3 methods give me the same response. I would appreciate it if you could maybe modify my workspace and upload it so i can have a look at it if possible. Only if you are able to though.

As for the footprint. I dont have the footprint for the LNA yet, which is why im using it as a short circuit in the layout. Im assuming i have to design the footprint myself as i contacted Hittite and they dont seem to have footprints available for the component. Is there a place that i could maybe download the footprint for the LNA? It is a 3 x 3 mm QUAD FLATPACK NO-LEAD (QFN) package.

 

[RF-OM]

I simulated your circuit with S-parameter files and get totally different response (high pass kind). Then I checked your filter file (filter alone). Your picture was very good but when I simulated it picture became different and high pass kind. It looks like something is wrong with your filter. I look on schematic and found that there are a lot unreal numbers like 0.36 mil length. This filter cannot be realized. Probably it is better for you to use your first interdigital filter. Try it with LNA S-parameter files and you should get better results.

Added after 12 minutes:

I also try to simulate your LNAs alone. Each of them has bog slope after about 1.5 GHz. When tey are connected together the slope is 10 dB from 1.4 GHz to 3 GHz. Is this slope acceptable for your project? Return loss also became not so good below 1.6 GHz.

 

[selva500]

Hello again,

It is interesting how you seem to get a high pass response with my filter as I have actually manufactured this filter already and the bench test still gives me a band pass response albeit with slightly higher return loss compared to the simulation. I'm not sure why this is happening as my simulations always return band pass response. The only problem i have when i simulate the filter and LNA together is the pass band becomes extremely narrow, Im not so sure why this is happening. Ideally i would like the pass band to be what it was originally without the inclusion of the LNA. As my filter is operating around the 2.2 GHz mark, the return loss below 1.6 GHz does not worry me too much.

The problem i am facing now is getting the layout footprint for the LNA. It is a 3 x 3 mm QUAD FLATPACK NO-LEAD (QFN) package. The package outline can be found here:
https://www.hittite.com/content/documents/package_pcb_layout/lp3_package_info.pdf
I cant seem to find the footprint layout for this type of package for the Genesys software (dxf/gerber format). Im not sure how to design the footprint myself as I've never been taught how to do so and have no experience in it whatsoever. I dont want this issue messing up my project. I was hoping someone could tell me where I could possibly find this footprint or maybe even help me out with it. It would be greatly appreciated![/u]

 

[webdog]

I had a quick go at the file... and noticed that the filter is extremely narrow, hence very lossy. Something has happened with your circuit. I did regenerate the filter and acheived 100 MHz b/w, then added the Hittite data from your de-embedded data, as I had no s2p files. Now I get the proper gain and passband!

Attached file is three screen grabs, first is what your circuit looks like, second is what I get when I recreate the filter using M-filter. Third picture shows how it looks like with the two amplifiers attached.

Note you cannot have the opimizing goals set your way when having two amplifers, as the gain will be so much higher, this is true also in the stopband. The circuit will collapse during optimization.

 

[selva500]

Many thanks for that. Im not so sure what u mean when u say that i cannot have the opimizing goals set your way when having two amplifers, as the gain will be so much higher, this is true also in the stopband. The circuit will collapse during optimization.

How do you get the response of the filter with the amplifiers attached without optimizing it. Or how does the circuit know that there are amplifiers attached to it. I thought the way of getting the filter response is to use the optimization feature. Is there another way of doing this w/o optimization? Also the insertion loss at the start of the passband seems to be high, is there a way to mitigate this at all? It may be helpful if you cud send your workspace if you dont mind. Do you have any suggestions regarding the footprint at all? Thanks again.

 

[webdog]

What I tried to say is that you cannot have the same stop band attenuation with and without amplification. You have to alter the optimization goals to reflect that you have added gain into the circuit.

After attaching the amps, you get the circuit response, pressing recalc button, and it will be updated.. you can then optimize the circuit, but using new goals.

As for the footprint, you have all the information in the Hittite document, it's just to copy that in the footprint editor.

BTW the gain from the two de-embedded amps do differ a lot in the passband... why? They should be pretty equal?? Could this data be the root cause of the poor match in low-end of passband? I have not the s2p-files for the Hittite components.

 

[RF-OM]

To selva500,

Sorry, I was too busy these days to check EDA site. I got high pass response by simulating what you gave me (if I remember it right). Regarding layout: I never create footprint in Genesys itself. What I did is to ask professional PCB designer create footprint for me and then transfer it to dxf file to use with EM simulators. Frankly speaking I do not remember how I use dxf with Genesys, may be with other programs. Usually you can find similar footprint in Genesys and try to simulate with this footprint. Results will be close if parasitic parameters for these footprints are close.

 

[selva500]

Hi

I have been trying to simulate an interdigital filter with the LNA attached to it. The linear simulation looks reasonably good but when it comes to the EMPower simulation things don’t go as well. Im not too sure why this is happening. Does EMPower account for the LNA attached to the filter because as I see it I don’t think it does. Is there a way I can set this set up? And Im not sure why the EM response is not so good either (S11 is very high and S21 is narrow bandwidth), I don’t see anything wrong with the circuit and I regenerated this circuit from scratch, it isn’t based on any of my previous designs either. I have attached my workspace and the s2p files for the LNA in the link below. I would appreciate it if someone could have a look.
**broken link removed**

Another question I have is when I finally integrate the LNA and connect it to the filter. Do I need some sort of impedance matching from the LNA to filter and back to the LNA again or I connect it straight to the feed lines (I don’t think the TL from the LNA will be the same width as the feed lines) or can I just omit the feed lines and connect the TL from the LNA straight to the resonators?


Lastly, the LNA is a No-Lead LP3 package. I assume there wont be any legs on the component to solder it on to the PCB. How do I then attached the LNA to the PCB. Is there a way to solder it manually or must it be done by a device of some sort?

Many thanks for your help.

 

[selva500]

Any thoughts anyone?