Controlled Impedance Routing - Page 1
Forum section: electronics / general

author: Gioreva
author_rank: Contributor
timestamp: August 01, 2018, 07:59:38 pm
content: Controlled Impedance RoutingI have to make USB 90 Ohm connection.I do not understand what I'm wrong.After design roule check, impedance is 259 ohm

author: rachaelp
author_rank: Unknown
timestamp: August 01, 2018, 10:02:19 pm
content: This will be a short reply because I’m on my phone sorry.You have a 2 layer board with no reference planes. You’ve also set your trace width to max 0.3mm. The tool can’t change the width enough to obtain the impedance you require. Google for some PCB impedance calculators and experiment with the microstrip impedance calculator with different with traces with/without a reference plane below and with the plane at different distances to get a feel for how the stack up affects the achievable impedance.If you want accurate impedance matching you’ll need to get your PCB vendor on board to help you specify the stack up to use.Best Regards,Rachael

author: Gioreva
author_rank: Contributor
timestamp: August 02, 2018, 06:01:08 am
content: I do not need accurate.I'm happy if DRC says 90 OhmI changed the maximum to 1 mm, but the routing is always similar and DRC always says 257 OhmsCan I try to reduce the clerance ?

author: Gioreva
author_rank: Contributor
timestamp: August 02, 2018, 06:05:51 am
content: Also with Clearance at 0.05, DRC always same, 257 Ohm

author: rachaelp
author_rank: Unknown
timestamp: August 02, 2018, 06:36:13 am
content: Your biggest problem is you don't have a reference plane. If you play with an impedance calculator you'll see why.If your bottom layer was a solid ground plane (which I know it can't because you need it for routing) then you'd get close to 90 ohms with 0.9mm - 1.0mm width traces on your top layer.If you had a 4 layer stackup with inner reference planes no more than 0.5mm away from the outer routing layers then you'd get 90 ohms with around 0.3mm width traces.Best Regards,Rachael

author: rachaelp
author_rank: Unknown
timestamp: August 02, 2018, 10:54:34 am
content: So I just reread your original post. You are doing USB so I think the differential impedance is 90 ohms which means the single ended impedance is 45 ohms. Here is a calculator which will help you calculate the parameters you need:https://www.everythingrf.com/rf-calculators/differential-microstrip-impedance-calculator

author: sdguy12
author_rank: Contributor
timestamp: August 02, 2018, 04:36:57 pm
content: I would recommend going with a 4-layer PCB. The cost difference between a 2-layer PCB and a 4-layer PCB is not that much. It is always better in general to have a reference plane for VCC/GND when designing impedance controlled traces. Remember that whenever you do a characterized impedance, you need to take into account the thickness of your dielectric material, the dielectric constant of the material, the width of the trace, and making sure that you have a solid plane underneath the trace for the return current since that goes directly underneath the signal trace. You can do that with a 2-layer board, but you have to play around with placement and routing on the bottom layer and your copper pour. Your life will be much easier if you switch to a 4-layer PCB using the a stackup like the following:L1/Top : SignalL2 : GNDL3 : VCCL4/Bottom : SignalAnd there are plenty of tools for figuring out the characteristic impedance of your trace to make sure it meets the 45ohm impedance that Rachael mentioned. I personally use appcad or saturnPCB.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 02, 2018, 06:27:34 pm
content: Are you using USB Full Speed, or High Speed?Full speed is little more than CMOS logic level, and doesn't care at all about traces this short. High speed is more critical, but won't mind a poorly matched impedance for trace lengths up to 200mm or so.Controlled impedance is impractical on 1.6mm two layer board. If you must, consider reducing board thickness to 1 or 0.8mm or even less (this reduces trace width below 0.5mm, still rather inconvenient), or positioning the receiver even closer to the connector, or using 4-layer construction.Note that Altium will not calculate the impedance without a reference plane. It doesn't know to check copper underneath or around a trace. Instead, it assumes a signal layer is empty, and a plane layer is solid copper. Better to calculate the trace width using an external calculator tool, and set design rules based on that.BTW, note that the USB common mode impedance is also specified. This sets how close the traces should be to each other, as well as their width, and the distance to nearby ground fill. Again, you don't have much option here, so follow one of the above strategies.Tim

author: Siwastaja
author_rank: Super Contributor
timestamp: August 03, 2018, 09:30:36 am
content: Since Altium cannot simulate or even approximate the actual impedance based on actual copper patterns, I fail to see the point in the controlled impedance routing function. Does it do anything else than what you can already do using any impedance calculator and just setting the width manually?

author: Gioreva
author_rank: Contributor
timestamp: August 05, 2018, 04:29:41 pm
content: TanksI can not use multilayer, I sell my card for € 40I use USB 1.0, the track is 5cm, I would say that I can limit my paranoia.I tried this calculator because it uses mmhttps://www.eeweb.com/tools/edge-coupled-microstrip-impedanceUsing 1mm trck, 1mm spacing, i have 4 value:Odd (Z): 74.9 ohms Even (Z): 104 ohmsCommon (Z): 51.8 ohms Differential (Z): 150 ohmsI have to obtain 45ohm for common and 90ohm for differential ?I have not 3mm of space for routing it, but i can on half lenght.

author: Gibson486
author_rank: Frequent Contributor
timestamp: August 24, 2018, 03:17:04 am
content: If you want controlled impedance, you need a solid ground plane under those traces. Usually this means you need a 4 layer board (at least...if your traces switch sides, you still need a ground plane right under those traces).Also, I only use those controlled impedance calculators to get me in the ball park of what trace width I need. Then I tell the pcb vendor what I need. I do this by making the traces a different size than the non impedance controlled traces. I add a note saying that all pcb traces with this width need to be xx ohm controlled impedance and that they can change the size to match their own stack up as long as it is a certain percentage of what I put on artwork.You could specify the actual stack up, but it will cost you more if you are just doing prototypes.

author: Gibson486
author_rank: Frequent Contributor
timestamp: August 24, 2018, 03:23:23 am
content: Quote from: Gioreva on August 05, 2018, 04:29:41 pmYou cannot do controlled impedance like that. You have some choices....make the traces as short as you can get it and hope for the best, put some buffer as your input and hope for the best, transcode the usb into a much more friendly (ie slower) protocol, go crazy with transformers.