Forum Discussion
Honored ContributorFPGA drive current effect on power draw in Cyclone IV
Howdy,
With the Cyclone IV FPGA, we have run into some issues with noise on Vccio and Vccint pins while using the 24 mA default drive current. I found an application note (http://www.altera.com/support/kdb/solutions/rd04062007_606.html?gsa_pos=1&wt.oss_r=1&wt.oss=power%20drive%20current) that mentions that the drive current affects the device power draw (obviously), but I can't find any quantification of this effect. Can anyone help me? I don't need an exact equation (although that would be nice) - even just a rough idea of the magnitude of the effect would be helpful. Thanks, Kathryn Turner13 Replies
Altera_Forum--- Quote Start --- Either if you have explicitely impedance-controlled boards or not, changing the I/O current strength effectively modifies the driver impedance. --- Quote End --- Exactly. Higher drive strength = lower driver impedance = less time required to charge the capacitance of the trace plus the load capacitance = faster rise/fall times = length of traces which must be considered as transmission lines is reduced. I'm aware that the discussion was about single-ended I/O standards, thank you. Perhaps I should have been more clear: A source termination resistor "might" be required at the driver to fully match the driver impedance to the transmission line impedance.- Altera_Forum
Either if you have explicitely impedance-controlled boards or not, changing the I/O current strength effectively modifies the driver impedance. It's a means to adjust the driver to match the trace impedance, which can be expected somewhere between e.g. 40 and 80 ohm for single ended traces with most multi layered PCB.
The discussion has been about single ended LVTTL/LVCMOS I/O standard, which usually can't be terminated at the load. In the speed range accessible by this I/O standard (e.g. 200 MHz), designed(calculated) rather than controlled(checked in production) impedances can be found with most PCB. - Altera_Forum
Kathryn,
Something you said in post# 7 caught my eye. You said that you were in fact having signal ringing problems, and not power supply noise problems? Can you elaborate a little? When you lower the drive strength of the I/O pins, you also lower the slew rate of the signal they are switching. Are you sure that the PCB traces are the correct impedance, and that transmission line effects aren't coming into play here? The rule of thumb that I use for determining if I need to treat a PCB trace as a transmission line is this: if the rise or fall time of the signal is less than twice the round-trip delay of the signal on the PCB trace (160ps per inch is good for back-of-the-envelope calculations), then you need to make sure that the trace impedance is controlled, and that the trace is also terminated properly. Ideally you would simulate the nets of concern in a high-speed simulator like HyperLynx, using your post-layout trace geometries and appropriate driver/receiver IBIS models before going to production. At any rate, if you can show on an oscilloscope that the signals ring too much at the receiver with the higher I/O drive-strength setting, but not with the lower drive-strength setting, then I would consider this problem solved. - Altera_Forum
Thanks very much, Jake, and danke schön, FvM. I really appreciate your time.
- Altera_Forum
With Cyclone II, the most likely failure mechanism is PLL unlocking caused by ground bounce or switching "noise" affecting VCCA. It's particularly a problem with PQFP packages and it's huge pin inductances. If lower drive strength doesn't help, reduction of simultanous switching outputs may be the only solution.
- Altera_Forum
There is absolutely nothing wrong with changing the drive strength to solve the problem and I say it's a valid solution and probably really part of the design rather than a problem. I mean, if I use the wrong drive strength on certain interfaces I can expect them to fail. If it were me, I would do some thorough testing just to make sure that there isn't something in the PCB design that needs to be fixed (poorly routed traces or stubs or something). If not, I'd change the drive strength and call it good.
Jake - Altera_Forum
also, I just noticed I inadvertently added two to our part number. It's a Cyclone II, not IV. Obviously, I shouldn't be posting while late to meetings, heh.
- Altera_Forum
It is ringing, not noise, sorry. And 24 mA wasn't a design choice - it's the default setting on the Cyclone IV. I don't think we realized the current was settable until we started looking for the cause (the problem didn't show up until after we did a board turn, but now that we know what to look for, we have found it on a couple prototypes). (In the "not helping" category, the engineer who did all the heavy lifting on this product for the last fifteen-plus years retired recently. We did ask him, and he thinks it's the simultaneous signal switching as FvM suggested.) My theory is that the bypass caps are right on the margin.
- Altera_Forum
Are you sure it's VCCIO noise that's causing your product to fail?
What are the main differences between this product and the previous version? Is it running significantly faster? Using different voltages? Handling more channels? The PCB must be different right? Just because a 24mA drive strength setting worked in one setting doesn't mean it will work in another. A 24mA drive strength on the I/O is too strong for many applications (most I dare say) and may result in significant ringing on the signals. Perhaps this is your problem rather than VCCIO noise. You should select a drive strength that gives the cleanest signal for your PCB design and termination scheme while still giving you adequate speed. Pounding all of your I/O with dramatic voltage swings and high dynamic current loads really isn't best practice. It may very well be that your new board is designed better than the previous one and you have lower parasitics on the signals making a 24mA drive strength too strong. Or it may also be that your PCB design is the problem. If it's really VCCIO and VCCINT noise that's the problem (I'd be surprised), this can be reduced by putting more effort into the design of your power delivery network. Basically you get noise on the rail because the power delivery network is unable to respond quickly enough to the dynamic current demands. It's impossible to remove all noise. Your choice of regulator, inductance, decoupling capacitor sizes, quantity, and types, PCB plane capacitance, via inductance all play a role in the regulator's ability to respond to those demands. Jake - Altera_Forum
Facing errors with higher drive strength is actually a kind of alarm sign. If you have a large number of synchronous switching outputs, some ground bounce can't be avoided. But you should check, if the ground wiring and supply bypassing is sufficient in your PCB.
