Where can i fabricate microstrip and help with GENESYS

2.2ghz narrow bandwidth filter

Hi there,

I'm designing a microstrip filter circuit as part of my final year engineering project. Im located in New Zealand and im wondering if anyone can help me point out companies that might be able to fabricate it. Preferably in the Australasian region (Oceania) but i wouldnt mind ones located in other countries as well. Without knowing what substrates they have access to it's quite difficult for me to design it accurately.

Another question i have is has anyone designed microstrip filters with GENESYS before? It's wizard like interface makes it easier to use but im wondering if there are any drawbacks from using it instead of designing the circuit with your own initial design(schematic based design). GENESYS is also capable of EM simulation which is quite useful as well but i haven't seen many people saying that they use this software which is why i asked this question. Lastly, GENESYS is only capable of exporting the design in DXF format. Would the fabricators be able to make the circuit using this. Is there a way i can convert it to any other more common file type?

Thanks in advance.

exporting s parameters genesys 2004

For a one off board your biggest problem is likely to be cost. You may be able to use on of the companies that will process your circuit along with others to reduce the overall cost. There are a few in here Europe and no doubt in Oceania as well.

As to material if you are going to use a 'microwave' ie not FR4 substrate that will make it even harder. You could etch a board yourself, there are a number of sites showing how to do this. With care very creditable results can be obtained.
You may be able to get a sample of the material you need form your local distributor. Manufactures such as Rogers, Arlon or Tachonic do some times give away small sheets of material, after all you may just use them when you start working in industry.

BY the Genesys wizard I assume you mean the microwave filter synthesis module. It uses the standard polynomials so should be no worse than something you design by hand, it just does it quickly and allows you to change things around to see what happens. It also creates the layout for you which is handy. When you have a layout I would recommend that you simulate it with one of the EM packages to get better accuracy. I don't have the Genesys EM simulator here but it does make a difference in Microwave Office.
Form discussions with others who use Genesys it is reasonably accurate, ie no worse than any of the other packages out there.

As to exporting the layout, just choose File >Export >Gerber File, It worked for me this morning. If you need to view the gerber to check that it is what you want there are many free gerber viewers available.

Peter

genesys microstrip

Many thanks for your help Peter.

I realise that cost could be an issue but we have a small amount of budget that we are allowed to spend on our project. Im not sure if it would be enough. I'm hoping some companies would provide a prototyping service. Would you be able to name me some companies so that I can make some enquiries. Searching on the internet hasnt been fruitful so far.

Im experiencing quite a bit of losses with the Fr4 material as my center frequency is 2.2 GHz. Is FR4 suitable to use with this type of frequencies? As to etching the board yourself, is it possible to do this with regular PCB fabrication techniques?

Sorry, i did mean the microwave filter module in GENESYS.The GENESYS EM simulator is called EMPOWER. Im not sure if its any different from the SONNET one in ADS as they seem to originate from the same company. Would there be a significant difference with the different packages, as my university has limited resources and it's difficult to get hold of different softwares.

Lastly, when exporting the layout. Can packages like MWO import gerber files so that i can do the simulations using it?

Thanks again for your help and I would greatly appreciate if anyone else could contribute to this thread.

impedance matching in genesys

Hi

Just a remark.
Genesys EMpower is using a grid for simulation and layout, which is different compared to ADS Momentum. In short Momentum is more precise because it generates an adaptive mesh.
But depending on geometry and frequency EMpower is satisfactory.

In the newer versions of Genesys, they have incorporated the Momentum from ADS. Thisis called Momentum GX.

Regards

microstrip layout design from scratch

One name that comes to mind is PCB Pool, I've seen their adverts in Electronics Weekly, but have no experience of their service. They seem to be geared around FR4 as I expect will most other manufacturers. When we have had prototype boards made at work the cost has been quite high as we are having to pay for the processing of a complete panel; there aren't many others wanting to process the materials we use, even though most of the substrates we use are FR4 process compatible. If you decide to use a PTFE loaded material, they can be difficult to process so you may have trouble finding someone who can do it.

As for making your own I know of people who have made boards for use at 10GHz and above at home using ferric chloride and iron on transfer material. There is a wealth of information if you Google DIY PCB or home made PCB or similar you should something. I would recommend a photographic technique, it should be more accurate.

FR4 is not the best material to use, its loss is high and results are not always very reproducible, it is not made to a tight spec like a microwave substrate. I've just made an end coupled filter from Genesys that came out at 2.75GHz, should have been 3GHz, but I did not EM simulate it. Its bandwidth is about 250MHz and loss about 6dB. I can live with that in my application and it was just an experiment to see if Genesys took into account the capacitors pads it adds to the lines; it looks like it doesn't.
Too get the loss down you could try suspended substrate, but I've not had much success with getting Genesys to synthesise a filter. It can get a bit large as the dielectric is partly air.

I don't think that you will notice that much difference between the EM simulators It seems to be mostly down to user interface, speed and small differences in accuracy; after all it would soon get around if any one of them was particularly inaccurate. Some of my colleagues have had good agreement with EM simulation and real life both Microwave Office and Sonnet Lite. Like all simulations the results are only as good as the data you put in.
You could give Ansoft Designer a try, the do a free student version, It has a filter design tool and I think it also has EM simulation.

No one here has managed to get gerber files into MWO, so it looks like it might be difficult, though if you have EM Power then it should not be necessary, just simulate what Genesys generates.

Peter

Thanks again guys. I will take heed to your advice and see what transpires. Ill have a read on manufacturing my own PCB and call up some PCB manufacturers to see what they have to say. Will also contact some material providers to see if i can get a sample or buy a small amount. I'll post any updates or further questions i have here. If there's anyone else wanting to input anything else please feel free

Selva

No one here has managed to get gerber files into MWO

Click to expand...

I have done it several times, of course I have their add-on software to do it. I used it primarily for checking power plane resonances by using a coarse EM grid. AWR has a new gridless simulator coming out so that would be more suitable for importing PCB artwork.

Just a remark.
Genesys EMpower is using a grid for simulation and layout, which is different compared to ADS Momentum. In short Momentum is more precise because it generates an adaptive mesh.

Click to expand...

No, Momentum does not have the dynamic range of the gridded MOM simulators such as Sonnet or EMSight therefore it will not be as precise, nor as accurate in the stop bands, since it uses numerical integration rather than FFTs. If your artwork is non gridded then Momentum may be more accurate, however it's usually easy to find a common denominator grid for traces and spaces so you would be better off with a gridded simulator to get accuracy and precision. Better yet try both and compare results. Note precision is not the same as accuracy. Precision is how many decimal places the result contains, while accuracy is how close the result is to a known-good standard.

Momentum would be better for antennas (with edge radiation) since it is an open boundary, while gridded usually has conducting sidewalls.

Hi again,

I have been reading through stuff about high frequency laminates. Roger's actually has a university program that they support which is good. I have a couple of questions regarding this laminates though. Ive also emailed the Roger's Technical support people but i thought i would ask here as well. The substrate i'm keen on is RO4003C as its FR4 process compatible. Hopefully it will make fabrication easier. My queries regarding this are:

1. I would like to know if this laminate comes with a copper layer that I can etch off for my circuit. I have read that the laminate can come with 1/2 or 1 oz copper cladding but I have also read in the fabrication section of the RO4003C that 'No special treatment is required prior to copper plating'. This confused me whether the laminate comes with one or do I have to plate it myself. Also if it does come with plating, is it on both sides of the laminate (ie can i use one side as the ground plane) or do i have to use an FR4 board with a ground plane as a base which would require me to acquire some prepreg as well i believe?

2. Is it possible to get the laminate with photoresist already applied on it as a lot of PCB manufacturers here dont have the facility to apply resist.

3. Next, I was hoping you could explain to me what the effect the difference in thickness of the substrate and the amount of copper (1/2oz or 1oz) will have on my circuit. I read that the difference in thickness changes the bandwidth value. How would I know the optimal value for these two variables that I require to give the best performance for my filter. Or is it completely up to me and I have to input the substrate parameters into the simulation software (I'm currently using GENESYS) and it will give me the layout corresponding to different values of the substrate parameters. Also could you tell me the difference between rolled copper foil and electrodeposited ones.

Hopefully some of you could help me out with these questions. It would be much appreciated. Thanks a bunch.

Selva

Added after 12 minutes:

Another thing I'm concerned about is the filter design itself. I have done simulation of a 3rd order Interdigital bandpass filter. Center freq = 2.205 GHz / Bandwidth = 200 MHz. The thing im worried about is the amount of reflection back from the input port. I have attached the EM simulation results I got from EMPower. Would anyone be able to tell me if its feasible to fabricate the circuit with this type of result (ie would it work alright?). And is there a threshold of some sort that i should be looking for when it comes to reflected power (S11). Btw, its the graph is an S parameter analysis. Red being S21 and and blue is S11.

Lastly, i have also attached the layout design produced by GENESYS. What i want to know is if there should be pads for the connectors to be soldered on to when the circuit is completed. How can i add them to the layout and would this extra copper pads affect the circuit response somehow.

Please refer to attachments.
PS: This isnt my final design as I havent finalized my substrate yet. I just wanted to try things out and find out as much as possible before i start on my final design.

Thanks again.

RO4003 is as good a choice as any for what you want, we use it here for quite a lot of circuits up to 10GHz or so and it works quite well.

If you ask for a sample it will come as double sided board. You can get just the core material, but usually only a PCB house would be doing that.

I don't know of anywhere that would supply it ready coated in resist. PCB manufacture starts with the bare board and photo resist is applied as and when needed for each stage of the process. You can get spray on resist from the likes of RS Components and Farnell. We use a LPKF milling machine here for small prototype circuits.

The substrate thickness and copper thickness is your choice, subject to what is readily available of course. Set these to get realisable circuit values and acceptable loss.

The FR4 that you usually get is rolled copper. If you peel it off you can see the glue. The better substrates are electro-deposited and cost more; I've never seen other than rolled FR4.

As a first cut what you have is not too bad. You could manually optimise the dimensions and get a better input match, or set up some optimiser goals and let the software do it. If you are not doing anything special with this filter i.e. there are no long cable lengths and you are not using wideband modulation then I wouldn't worry too much about the match at this stage. If you have the system simulator you may be able to investigate the effects of mismatch.

TL1 & 6 are the 50 ohms transmission lines that connect your filter to the rest of the world. To test the filter connect a coax connector between the groundplane and the end of the track. I would us a SMA with the inner laying on the track and the outer soldered to the ground plane. The through hole types with 4 ground pins can be pushed over 1/16" FR4 and make good enough contact for a quick check without having to solder them.

If you have other stages place them on the same substrate at the connection points.

Peter

Thanks again Peter.

Im currently communicating with a Rogers rep to get some RO4003 samples sent to me. I'm not sure as to what method I'm going to use to fabricate my circuit, either etching or milling. Would milling affect the performance of the circuit much as it obviously isnt as accurate as etching.

I'm not really going to be doing anything fancy with the filter. It's meant to be part of a low noise amplifier where there is a first stage of amplification then the signal passes through this filter and then there is a second stage of amplification. I've actually increased the bandwidth from what i really want. The narrower the bandwidth the better for my purposes but i have to compromise somewhere. I'm going to run some simulations with a smaller bandwidth and using the RO4003C substrate tonight or tomorrow. I will post the results up again to see what you think.

As for the input/output of the filter. What i was curious about is if there should be some kind of footprint for the SMA connector to be soldered on to or does it get soldered straight onto the TL1/TL6 lines. There is an option in GENESYS to place port footprint. I'm wondering if i should do this or not. Thanks for your time again. Its much appreciated.

Selva

First of all I want to tell that Genesys is the best tool for microwave filter design. Actually it produce results that about 1.5 to 2 % off from bench test. Next is HFSS with about 5% accuracy in very best case. The serious problem in such design is to find good PCB manufacturer who is able to keep required accuracy. It should be no more than +/-0.5 mil accuracy for trace geometry and +/-5% for board material dielectric constant. Plating absolutely unacceptable for filters! You design copper thickness as 0.5oz (0.685mil) but in reality it will be at least 2.2mil with plating. The best is Rogers with rolled copper because rolled copper has better roughness. But even FR4 may provides good results if vendor is able to keep dielectric constant as it required. The actual loss of the filter depends more on bandwidth than on material dissipation factor. If you need very narrow filter forget about low loss and FR4 probably will be good from the loss point of view. But when your filter is broadband the quality of substrate material become more important and here Rogers may be a good choice. In any case try to keep traces as wide as it possible and spacing as well. It will help with manufacturing inaccuracy.

Next point. Your pictures from Empower simulations are not right. You need to move feed lines away in order not to overlay metals. You also have a negative length of traces, which is definitely wrong. Next - there should be end terminations at the end of the traces, but you have another terminations. I do not know your design, but it looks suspiciously, please check all these points.

When you finalize your design, try to simulate it with different grid spacing. Often it helps to avoid mistakes. In your case vertical spacing can be big, whereas horizontal is better to keep not more than 5 mils. Try to match the greed as much as possible. And last: finding good vendor for PCB is one of the hardest task in microwave filter design. You need to talk to these guys and verify every small point in the board. Will they able to do it or not. When you get the board check it with microscope for all dimensions. Price may be high, but filter boards are complicated and here is almost nothing what you can do.

Hi there,

Thanks for your input. From what ive the Rogers representative has told me, the supply the laminates already pre-plated so I dont think the thickness of the copper would be an issue. Im trying to get a 1oz copper and 0.032"(0.813mm) dielectric thickness. I would expect the specs of the board that they send to me to be something close to this as thier error margin seems to be very low 1-5% at the most, even the dielectric constant only has an error of 2%. The only thing that the PCB manufacturer has to do for me in my case is get the trace geometry right as u said and etch out the circuit pattern according to my measurements. My original aim was to get a bandwidth of 10MHz but after researching i think this would be quite complicated for a student project as we dont have much facilities and fabrication techonology so i would be happy with 100MHz. I think the losses would be important in my case as it is going to be part of a receiving end of a satellite signal as part of a ground station.

What im concerned about now is yr comments abt my simulations being incorrect. I have a couple of questions regarding this as im not sure if understand completely what you are trying to tell me. I hope you could clarify this further.

1.You need to move feed lines away in order not to overlay metals.
-- I assume you are talking about TL1 overlapping with TL4 and TL6 overlapping with TL5 in the layout. Im not sure about this as this is the layout GENESYS automatically generated when i put in the filter parameters. The green dots in the layout snap and lock to each other. If i move it it there is a line displayed showing that it is meant to be connected at the green dots.

2.You also have a negative length of traces, which is definitely wrong.
-- Again im unsure about what you mean by negative length of traces. Could you please describe this to me in more detail and possibly point out which lines you are referring to.

3.Next - there should be end terminations at the end of the traces, but you have another terminations.
-- What do you mean by end terminations. Again I was working based on the assumption that GENESYS would provide me with the right layout for the filter design i required. All the traces are grounded. And the input/output have EMports attached to them for simulation purposes. If there is something not right about this, please do point it out.

Hopefully u can elaborate on some of the points you have stated as it will definitely help me to get the filter right the first time around and not go around in circles especially when time is tight. It is due in about 2 months and i have to allocate time for the samples to arrive, which could be 2 weeks or so, and for manufacturing. I'm extremely grateful to all the people who have been advising me as the staff in my uni are not very experienced with microstrips so this board has been of much help to me. Thanks.

1. Overlapping. You are right: TL1 and TL6 overlaps with resonator traces. You need to move them apart to the edges of traces. When metals are overlaps simulation may give wrong result. This is what Randal Rhea, the former owner of Eagleware and the author of this filter design module, told me in our discussion. I checked it for many years and this is the true. I think here is not the best place to go deeply into EM simulation issues to explain this phenomenon. Please trust me just on words.
2. On your picture TL4 and TL5 have negative length. Unfortunately it is happen sometimes in Genesys M-filter module, but it is wrong. Try to play a bit with variables and you will find another combination without negative lengths. Sometimes, especially when negative numbers are small you may set them equal to zero.
3. Your first and third traces must have end terminations (capacitive) that are almost always slightly wider that the trace itself. It is done to compensate an effect from tapping.

You may play with all these numbers without EM simulation until you get good response from the filter. Use about 15% higher frequencies because after EM simulation they will be lower for about 10 to 15%. After you get good response, start EM simulation. Try to have as much metal on the grid as it possible. For example, program gave you trace width about 41 mils. Use 40 for 10 mils grid and your trace width will be exactly on the grid. The same is true for spacing and trace length. When you will get good results with EM simulation you can adjust geometry. Try different grid spacing. For example 20mil for vertical and 5 for horizontal, then switch to 10 mil vertical and 5 (or 2.5) horizontal. You must get similar results. If there a big difference something is wrong. You have only three resonators, so EM simulations should be easy enough for any experiments.

Good luck with your design!

Hi again,

Thanks for your advice. I will try and do what you said and definitely try simulating it with different grid sizes as well. I see what you mean by negative traces now. One thing im still not sure about is the capacitive end terminations, how do i include them in the layout?

Is there some option in Genesys that will allow me to do this or do i have to do it manually? If i have to do it manually how big should the termination be?

Would it be located where the ground is currently on the trace or on the other side of the trace?

This is my prelinimary design, with 200MHz bandwidth. Im thinking of setting the bandwidht to 100MHz and making it a 4th order filter. If i do this, would the end terminations still be on the first and last resonator trace again or on another trace?

Thanks for your time yet again.

Terminations usually chosen by Genesys in time of filter synthesis. Probably you need to start design again from scratch. You also may include these two termination by yourself from the layout elements, but better to allow program to do it. Without good experience with filter design and with manufacturing you may expect an accuracy about 10%. It means that if your central frequency is 2400 MHz you easily can get it somewhere between 2150 and 2650 MHz. In this case having filter very narrow may be not possible. If you will be very accurate you may get 5% accuracy, but it is better to expect 10%. You may slightly tune filter with Exacto knife, but this is the last measure.

Good luck!

Hmm, the thing is i have played around with Genesys a couple of times and when i choose an interdigital topology the circuit layout is always similar to the ones ive posted. I havent yet encountered anything with a different type of termination but maybe there is an option for it somewhere. Would making the filter a 'tapped' one make any difference in this case because thats what I'm doing as i read somewhere that its a better option. Cant remember why exactly. But in any case I will try and tinker arnd with the circuit to see what i can acheive and I will post it up here again as soon as I have something.

Hi

Just a comment on the overlapping traces. I think you need to add some tee-junctions to make it right.

Regards

You need to go through all the setup options in Design section. I did some simple design for you and made all screen shots. I hope you can easily repeat it. This is only schematic simulation, not Empower. You can do it by yourself. When I stated to do design I get negative lengths for LA and LB (terminations). I just replaced negative -18mils with 10 mils and then adjusted Lbot and Ltop to get right central frequency and good matching. Substrate is Fr4 with rolled copper from Genesys library. Try to play with Rogers too.

I hope it will help you.

I am sorry, but I forgot to tell you that feeding line may too wide. On layout that I sent you they ate very wide. In this case it is better to connect them through tapered line. The widest side should be equal to feed line width and the narrow side may be about 20 mils (0.5 mm). The angle of the taper may be about 45 degrees.

Hello all,

I have managed to design several circuits and bench tested them. My best designe is based on the hairpin topology. At my center frequency (2205 MHz) im getting an insertion loss of about -4dB. Based on this my -3dB cutoff points, which will be -7dB in this case are 2155MHz and 2225MHz which gives a passband of 70 MHz. My questions are:

1. Is the -4dB loss acceptable for a microstrip filter? Is there a way I can improve it at all. All my designs came up with a loss of at least -4dB. I would like to minimize the losses if possible.

2. Is there a way of reducing the bandwidth of the filter without increasing the losses? When i simulated the design with a lower passband the losses increased, I assume this is normal and there is a tradeoff between both factors.

I would appreciate any comments/suggestions. Thanks.