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

Req: PCB Material for 5.6 or 5.8GHz Design

Status
Not open for further replies.

Rayengine

Full Member level 5
Joined
May 18, 2001
Messages
287
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,298
Location
Hong Kong
Activity points
1,737
rogers pcb material

Hi All,

We are currently engaged in 5.8GHz design, what materials is most preferable in the frequency ? We planned to use FR4 with microstrip line.

Any valuable experienced idea!

Rgs

Rayengine
 

WYL

Junior Member level 2
Joined
Dec 31, 1999
Messages
22
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
China
Activity points
73
how to design pcb materials

Yes,you can use FR4 to 5.8Ghz microstrip line,it's no problem.



Regards,


WYL
 

mwpro

Member level 4
Joined
Apr 20, 2001
Messages
71
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
700
rogers 3000 micrstrip design

Agree. If you are doing lumped design, it is fine. However, if you are using distributed elements, be aware of the associated loss (1 dB or so).

Besides, I suggest you to look for thin dielectrics so that the line width are small and hence the junctions are small.

regards,
mwpro
 

nandopg

Full Member level 4
Joined
Apr 26, 2001
Messages
205
Helped
8
Reputation
16
Reaction score
3
Trophy points
1,298
Location
Over the Rainbow
Activity points
2,540
thermal analysis of pcb materials

For 6GHz design, the usage of lumped components should be made with extreme care, being necessary to characterize each component before use. Depending on the application this can be a true problem.
So distributed design or at least a hybrid design, should be regarded to implement the circuit structure and the choose of a good microwave substrate comes in to scene. Some good substrates can be regarded for 6GHz frequency range:

Rogers RO6305 - Duroid with er=10.1

Rogers RO4350 - er=3.48 (low cost). This substrate is more lossy than RO6350.

Rogers Ultralam 2000 - er=2.2-2.5. This substrate is teflon based, exhibiting an extremely low loss and reasonable cost. The problem is the difficulties to plating holes. If you choose this substrate you should ask to your pcb house if processing teflon based pcb is available.

All examples above are for substrates manufactured by Rogers and they are what I have been using for 6GHz designs. However there is a lot of other manufactures.

Hope this help you,

NandoPG
 

g579

Full Member level 6
Joined
Dec 31, 1999
Messages
322
Helped
19
Reputation
38
Reaction score
4
Trophy points
1,298
Location
Somewhere
Activity points
2,470
pcb teflon epsilon r

Depends on the design type.
Wide band low Q : FR4 can be tried
Filter, higher Qs : rather Rogers 4000 series, the same (low cost) technology as FR4 and material cost is in the low range.
Hope it helps too.
 

freddy_microwave

Junior Member level 3
Joined
Jan 24, 2002
Messages
28
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Location
the wild east
Activity points
152
pcb roger layer ghz

Would not use FR4 for any 6GHz design. If you have no problem
with the losses be aware that the eps_r drops down with frequency.
Its at 4.2 at 2 Ghz (ca. values) coming from >5 at DC. May measure
it. Otherwise RO4003 is the best choice with care to the costs.

Freddy
 

toonafishy

Full Member level 6
Joined
Jun 18, 2002
Messages
369
Helped
38
Reputation
76
Reaction score
12
Trophy points
1,298
Location
Earth
Activity points
3,187
roger pcb microwave design

If the dimensions/trace lengths are very short, FR4 is okay. But if they are longer, then there is a loss problem. Rogers 4000 is nice to use but you do not have to do all layers in it. To save cost, I sometimes do the top layer in FR4, the next layers in Rogers and the bottom layer in FR4. This works pretty good and is alot cheaper than doing it all in Rogers. You can easily put the specs for FR4 or Rogers in your EM simulator and see if you can live with the losses.
 

g579

Full Member level 6
Joined
Dec 31, 1999
Messages
322
Helped
19
Reputation
38
Reaction score
4
Trophy points
1,298
Location
Somewhere
Activity points
2,470
ultralam 2000 temperature

toonafishy,

Seems to be a bright idea.
Question is wheter in the mixed FR4 and Rogers layers case aren't there (from the different thermal expansion coefficients) mechanical problems for a wider temperature range ?

g579
 

mwpro

Member level 4
Joined
Apr 20, 2001
Messages
71
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
700
rogers cte fr4

CTE of FR4 and Rogers 3000 and 4000 are quite close.
Mix them together is quite common.

regards,
mwpro
 

toonafishy

Full Member level 6
Joined
Jun 18, 2002
Messages
369
Helped
38
Reputation
76
Reaction score
12
Trophy points
1,298
Location
Earth
Activity points
3,187
rogers 4000 pcb

Your observations are correct but I haven't had any problems with this. Lately, I have been using this method on RFIC production test socket boards. These boards fit in an HP84000 tester and test thousands of ICs per day. The FR4 gives the mechanical rigidity needed and the Rogers give the nice RF performance for testing. It seems to hold up well over test temp of -40 to +85 C.
 

VSWR

Advanced Member level 3
Joined
Feb 7, 2002
Messages
749
Helped
103
Reputation
206
Reaction score
23
Trophy points
1,298
Activity points
5,425
microwave design pcb materials

I have bad experience using FR4 at these frequencies. Epsilon-r as well as thickness is uncontrolled. I.e. high tolerances on these parameters gives offset of center frequency of sidecoupled microstrip filters, etc. In addition, the temperature coefficient of these parameters is large as well.

Go for Rogers substrates instead.
 

g579

Full Member level 6
Joined
Dec 31, 1999
Messages
322
Helped
19
Reputation
38
Reaction score
4
Trophy points
1,298
Location
Somewhere
Activity points
2,470
pcb material for ghz

toonafishy,

Thanks for your remarks. If you use it regularly with no problem on temperature change means the design idea is OK for practical purposes.
Thank you.

g579
 

Gemini1706

Member level 5
Joined
Jul 3, 2002
Messages
81
Helped
3
Reputation
6
Reaction score
2
Trophy points
1,288
Activity points
1,120
material fr4 epsilon

FR4 is total crap for RF.

Huge tolerence of Er is a big problem.
It changes from board to board, so you will get really poor yeild...

I would not recommend using it even at 2GHz :)
 

Rayengine

Full Member level 5
Joined
May 18, 2001
Messages
287
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,298
Location
Hong Kong
Activity points
1,737
fr4 epsilon material

Thanks for all valuable reply!

One more questions : If we still go FR4, but we choose multi-layer PCB (4-layer), what is the stack preferable (i.e the thickness of each layer).

Best Rgs
 

mwpro

Member level 4
Joined
Apr 20, 2001
Messages
71
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
700
epsilon fr4 frequency

I think the stacking thickness really depends on the prefered line width.

regards,
mwpro
 

Rayengine

Full Member level 5
Joined
May 18, 2001
Messages
287
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,298
Location
Hong Kong
Activity points
1,737
printed pcb filter 5.8ghz

mwpro said:
I think the stacking thickness really depends on the prefered line width.

regards,
mwpro
I knew that the fact that thickness depend on line width. As I really want to know that frequency dependent on the FR4 thickness, small thickness has minimize the loss, and I right ?

We also need to concern the rigid of board when applied in product if too thin thickness are chosen.
 

Rayengine

Full Member level 5
Joined
May 18, 2001
Messages
287
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,298
Location
Hong Kong
Activity points
1,737
pcb + rogers material

mwpro said:
I think the stacking thickness really depends on the prefered line width.

regards,
mwpro
I knew that the fact that thickness depend on line width. As I really want to know that frequency dependent on the FR4 thickness, small thickness has minimize the loss, and I right ?

We also need to concern the rigid of board when applied in product if too thin thickness are chosen.
 

VSWR

Advanced Member level 3
Joined
Feb 7, 2002
Messages
749
Helped
103
Reputation
206
Reaction score
23
Trophy points
1,298
Activity points
5,425
pcb material thickness tolerance

Rayengine, unfortunately you are out on deep water now.

Ask your board manufacturer of epsilon-r tolerances on the multilayer FR4 they will manufacture for you. I doubt they can provide these data for other frequencies than 1 MHz. Nevertheless, use these values for tolerance analyses in your microwave analysis program. You will be surprised of the result...

In addition, the manufacturer cannot keep individual layer thickness tolerances within sufficient ranges. Ask them for typical values and - again - use them for tolerance analysis.

How to perform tolerance analysis (e.g. MonteCarlo analysis) in your microwave program is often explained in the manual or through supplied circuit examples.


Rayengine said:
Thanks for all valuable reply!

One more questions : If we still go FR4, but we choose multi-layer PCB (4-layer), what is the stack preferable (i.e the thickness of each layer).

Best Rgs
 

g579

Full Member level 6
Joined
Dec 31, 1999
Messages
322
Helped
19
Reputation
38
Reaction score
4
Trophy points
1,298
Location
Somewhere
Activity points
2,470
what is rogers pcb material

Rayengine,

One remark or proposition.
If you are not sure about Er of FR4 at your frequency, you can easily measure it by a loosely coupled half wavelenght resonator you make on your FR4 material (you measure the resonant freq, and knowing the mechanical measurements you can calculate).
For further work you can use the same sheet of material with approx. known Er, and taking into consideration the dimensional tolerances.
g579
 

mwpro

Member level 4
Joined
Apr 20, 2001
Messages
71
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
700
pcb rogers material

Rayengine,

Yes, a too thin substrate has rigidity problem. But you may back it up by a thick layer of FR4 isolated by ground plane.

regards,
mwpro
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top