Which CAD/EDA tool to "invest" on ?

[nctnico]

Many people have done a great many things without SI, some quotes from Bob Pease come to mind.

However, Bob Pease never dealt with (for example) memories running at >1GHz where SI really matters. Being able to run a simulation of the signal integrity of a board can save thousands of euros/dollars on a board respin alone (without taking the costs of delayed sales into account).

[olkipukki]

Also, for those serious about high-speed designs, there is SI option for the Orcad Pro

I'm a bit lost here, is it part of OrCAD Pro or a separate package?

[asmi]

I'm a bit lost here, is it part of OrCAD Pro or a separate package?

It's a feature of SigXplorer (which itself is a part of Orcad PCB software package), but it's only unlocked if you have SI license option.
With Orcad, all license levels are physically the same product. They simply disable/enable certain features/functions based on what license you have installed/activated. Which is one of it's strength in my opinion, as you can start small (baseline Standard or Pro level) and add extra options and features as you need them, while still using the same basic software - so no learning curve, and no software installation/configuration is required - you just add a new license, and additional features are unlocked.

This is a bit of offtopic, but I think Altium should've done the same thing to create cheaper "editions" of AD instead of essentially developing the same thing tow more times for Circuit Studio and <whatever their free cloud thingy is called>. That way transition to higher level would be much more painless than it is right now.

[olkipukki]

I'm a bit lost here, is it part of OrCAD Pro or a separate package?

It's a feature of SigXplorer (which itself is a part of Orcad PCB software package), but it's only unlocked if you have SI license option.

Are you sure about a separate license?

Starting in 16.5 and continuing to the present version (16.6), you can perform signal integrity (SI) analysis from your OrCAD PCB board file using only your OrCAD PCB Professional license (no special SI licenses needed!)

The SigXplorer tool which is using your OrCAD PCB Designer Professional license will open with a copy of your net’s topology.

https://resources.ema-eda.com/blog/how-to-perform-signal-integrity-analysis-on-nets-in-orcad-pcb-designer-professional

[asmi]

Are you sure about a separate license?

SigXplorer is available at all license levels (even the most basic Standard), but it has some features disabled at lower levels. At standard level, as far as I remember, only pre-route simulations are available. At professional level (which is what I have BTW) you can do everything except parameter sweeps. That last feature requires SI license. They might've changed things in version 17.4, but I only have a license for version 17.2.

[ElectronRob]

And neither do I thankfully

You've also kindly made my point for me, high speed digital design is a great use of SI, using it for everything all the time is not.

[asmi]

You've also kindly made my point for me, high speed digital design is a great use of SI, using it for everything all the time is not.

And you'd be wrong. Crosstalk can become an issue even in low-speed designs. The classic example is reset line which goes along some signal line with sharp edges, and in certain conditions enough of a signal can couple into reset line to trip the processor into reset. I've seen few boards which have this problem, and one of those was designed by no other than yours truly - that was back when I, just like you are now, thought that crosstalk is only a problem for high-speed lines. Well, I learnt that lesson the hard way If you don't want to repeat my mistake (with literally weeks of debugging and banging my head against the wall before I was able to figure out what the problem was), I'd recommend you to pay attention to this problem. This is especially so if you use modern low-power low-Vcc devices, as the lower the interface voltage, the lower the gap is between logic zero and one, and less of a crosstalk is required to trip the circuit. You can actually calculate crosstalk using free Saturn PCB Toolkit - play around with it, and you will see it doesn't take that much to cause problems, as modern chips have very sharp edges, even cheap STM32F4 MCUs can output signals with rise time of only 2.5 ns, more advanced MCUs and pretty much all FPGAs can reach sub-nanosecond rise times.
Just for reference, at 3.3 V Vccio and typical 1.6 mm two layer FR4 PCB (Er=4.6), for 1 ns rise time signal it takes less than 10 mm of coupled length at 0.25 mm apart to have 3.2 V crosstalk spike in adjacent trace, for 2 ns the coupled length is 15 mm for the same spike, for 5 ns rise (which AFAIR even atmega328p can reach) you need about 40 mm of coupled length. As you can see, it doesn't take all that much to cause issues which are going to be *extremely* hard to debug because presence of debug probe and even your hand will change the behavior (because it will change load capacitance of the trace).

[ElectronRob]

Hi,

Thank you but I think we are drifting a little far from topic now. I understand what cross talk is, I understand what I like to use sim for. I am not a perfect designer (who is?) but I have been designing a variety of solutions for some 15 years now, even the worst designer would be familiar with cross talk by now I mostly design very low noise or very high current circuits, switching 1500amps through an Hbridge does indeed present some problems with control lines etc.

High speed digital IS a great application for SI - why am I wrong there. I already calculate crosstalk for anything important and guess what, I use Saturn PCB I did say thats what I did earlier.... you seem to think im disagreeing with you, I am not but I am also not asking to be educated here - but thank you for trying, I think you are being nice about it.

I am sorry to hear that you spent weeks of debugging, I would suggest you purchase some good test equipment and a good differential probe (or several!), I would also suggest that you slow any line down which doesn't need to be fast, do you really need that 2.5nS rise time to turn on that LED?

 

[Shadowfire]

I made the decision to go with Orcad PCB Designer Professional and added the Pspice option, instead of Altium Designer.

In the end the two packages seemed closely matched; it was primarily due to being the same package as I use at work, but there were a few other minor factors pushing me in that direction.  Keep in mind that I haven't actually used Altium (although I have used CircuitStudio), and that I've spent 5+ years using Orcad at work;  I'm going by the documentation that Altium had on their website.

1. XSPICE vs PSPICE:
PSpice seems to actually have component manufacturer support (models).  No need to go get an NDA with every component manufacturer to get an unencrypted model (which you will likely not get if you aren't working for a company).  Additionally the Pspice smoke option doesn't seem to have a counterpart in Altium.  (Yes you should be designing things with adequate safety margins... but changes happen, and isn't it better to not have to recheck everything manually because you made a minor change?  Smoke allows you to see problems with a cursory inspection.)

2. Signal integrity:
Both packages seem close to on par with IBIS models/signal simulation (The only significant difference I noted was that Orcad models the vias, but Altium does not.)

If Altium only generates text reports for SI, I can completely understand why asmi think that Altium is junk (although I think that the term "primitive" is probably more accurate).
The SI visual analysis tool (for impedance and crosstalk) in Orcad PCB Editor is **wildly** better than just having a text report with calculations & coordinates.

Basically, it seemed that wherever I looked and found an appreciable difference, Cadence's solution seemed more time-efficient.

[olkipukki]

I made the decision to go with Orcad PCB Designer Professional and added the Pspice option, instead of Altium Designer.

How much did you pay for the option if I may ask?

[Uky]

Things to consider when deciding what tool to "invest" in:

1. Are you considering a career as a professional PCB Designer?

The PCB designer community is getting older and many young are not that eager to pursue
careers in professional PCB design. This is IMHO partly because PCB designers are often considered
"draftsmen" with little or no esteem amongst design engineers.

Having one foot in the electronic design community and the other as a CAD engineer could prove
to be difficult. However - A skilled PCB engineer that masters a complex tool with good
knowledge in signal integrity issues as well as complex PCB systems will be saught after.

2. If an entrepreneur, do you forsee that your business will grow in terms of product
complexity? Choosing a tool that you can grow with means that the most important
part of the investment can be maintained: The libraries. Being (reasonably) experienced
with Cadence OrCAD/Allegro, it is possible to start with an inexpenceive version and
later purchase performance upgrades. The libraries will stay intact. No need for changes.

I guess that the more expenceive competitors provides this option as well.

3. Need for technical support? Is there any 24/7 support service if your design
crashes for whatever reason?

4. Any need to interact with other businesses that uses different systems?

I have seen questions such as "How to produce a net-list for a (competitors) PCB Editor".
Previously, OrCAD could produce a lot of netlist formats even for defunct
systems such as "EEDesigner" (DOS-based), but with 17.40 this option has been lost.
And it is of course understandable. What is important however is the possibility to
import other vendors schematics and PCB-files!

5. Are there possibilities to interact with mechanical tools?

Personally, I consider AutoCAD to be Cadence' "best friend" because of the flexibility to handle
arbitrary shapes of footprints and board outlines. Since 3D has become important, having
an interface to import and handle STEP-models are becoming more and more important.
Hence also knowledge of softwares such as Inventor/Solid works etc is an asset.

6. Are there possibilities to produce output formats such as IPC 2581 and ODB++?

There was a "fight" some years ago between Cadence advocating 2581 and Mentor, advocating ODB++ (which they owned
thanks to the purchase of Valor). (It seems that the dust has settled now)

If the answers to the questions above is no or not likely, I would definitly go with free software.
I am however watching KiCAD since I see this tool getting more and more competent
and gaining momentum.
The question is what happends if the driving forces looses the will for whatever reason.

This is a risk with any software but IMO, it is less likely for the big guns.

[Shadowfire]

Just wanted to chime in that the Orcad PCB designer pro package has an astounding setup for PCB impedance and crosstalk analysis.  (It's apparently a cut down version of their Sigrity tool, but oh my god is this thing an amazing time saver.)

Lay out your board.
Do your initial routing.
Check your routing SI with the topology explorer and fix any reflection/routing or termination issues.
Use coupling (crosstalk) vision to space out your traces and minimize crosstalk.
Use impedance vision to find impedance discontinuities (vias on plane splits, adjacent vias, traces crossing over plane splits, traces running adjacent to copper pours, etc).  This will also show you if you missed any impedance constraints in constraint manager.
Final routing SI checks with topology explorer.