Poking and prodding allegro - erm, what?

[daqq]

Hi guys,

So, I'm trying out allegro. At a job I have been a long time OrCAD Layout (not the current layout, the old Layout) user and, while it had its quirks (which, during several routing sessions got it named 'unholy monstrosity that will be uninstalled with glee and the install CD will then be purified by holy acid') it was workable. Not awesome, but workable, particularly, since the software was from 2005.

So, I'm trying out the new stuff - the schematic part is pretty much the same. A small change here and there, but the main functions are pretty much the same as far as I can tell... now the Layout, Allegro...

Disclaimer: I've only been using this for a day or so, as such, it's possible that I missed some stuff. For stuff I missed I apologize, please correct me where I'm wrong. But I'm pretty annoyed by now.

So, as far as I can the damn thing does not have a PCB footprint library browser. It's got a load of files, in which individual packages are stored and you can open them, but that's that. There is a work around, where you can place something manually and 'browse' the available footprints, but WTF? Layout had a simple browser/editor that worked.

Pads editor: So, apparently a pad is stored not in a component, but rather in its own library/file.

So, the process of creating a component should work as follows: I create my pads in one application. Then I create my footprint using the predefined pads (which if I need to edit I have to start up the different application again and synchronize it somehow). Then when I want to view the footprint some time later, I can open the file (which will sit among a gazillion other files). When I want to browse the available footprints, I can always use a bad workaround.

They have their own language, which calls traces CLines, etch or something. Awesome.

The keyboard shortcuts are not the same as in Layout... that's OK, I don't expect to have two conceptually very different systems sharing the same set of keys... but apparently you can't bind single letter keys (such as I = zoom, O = unzoom, G = unroute trace segment) which is annoying. Instead, when you press those, they are entered into a console.

I have yet to find a method to unroute just a bit (segment) of a routed trace.


It seems, well, very non-intuitive. The whole user interface seems kinda strange. I never thought I'd say this, but the old Layout seems more friendly. It's just the demo so far...

What is the local opinion on the whole Allegro thing? Is it worthwhile to investigate?

Thanks,

David

[Alex Eisenhut]

"Pads editor: So, apparently a pad is stored not in a component, but rather in its own library/file. "

Of course, how else can you re-use it in other components? It's a powerful tool.
Establish a consistent set of house rules here, like imperial or metric, etc.
Allegro has a path to find padstacks, try to keep things simple by keeping padstacks in a separate directory.

Allegro is such a complex and powerful beast it's almost impossible to grasp all of it in a few days. Even after years I'm still going "oh".

But keep in mind it has evolved over decades and has roots in workstations, so it'll have picked up pretty quirky ways of working over time.

It *is* overwhelming, because you thought you bought a bike and are now sitting in the cockpit of a 747.

"They have their own language, which calls traces CLines, etch or something. Awesome. "

Of course, so does Pads, or Altium. Just learn it, and that's it. Sure, there's subtleties and sometimes frustrating inconsistencies.

"The keyboard shortcuts are not the same as in Layout..."

So? Make your own. Allegro has its own command line. Go ahead, type alias and press enter.

You'll see a list of aliases... create your own.

Soon you'll have little script files you tie to specific keys and BAM, things are flying all over the place.

A footprint viewer is in the schematic tool. The only way to view footprints in Allegro is by opening the symbol. You can of course also run a Free Physical Viewer (no license needed) to open symbols.

Feel free to ask me anything.

Also, consider keeping a written journal of your discoveries. It sounds trite but it works.

Um, what kind of layouts are you considering?

[daqq]

Of course, how else can you re-use it in other components? It's a powerful tool.

Well, I'm OK with the separation of schematic symbols and footprints - it's preferable to how, say, eagle does it. What's annoying is that there seems to be no reasonable way to browse and view them, like there is in the old layout. I'll look into the Free Physical Viewer.

Um, what kind of layouts are you considering?

Other than this (OrCAD standard) we were considering Circuit Studio. If you mean what level of design complexity, well, 2-6 layer boards, nothing super complex.

Feel free to ask me anything.

Thanks for the offer! So, here it comes:
Is there any way to unroute just one segment of a drawn trace?
Is there any way to quickly rotate a component by 90 deg without all the mouse clicking the menu option?
What's up with the via system? Again, I have to have a library of prebuilt vias? What the hell?

[AndyC_772]

Is there any way to unroute just one segment of a drawn trace?

Yes, right click and 'oops'. From memory the default shortcut is F8.

What's up with the via system? Again, I have to have a library of prebuilt vias? What the hell?

Yes, that's how it works, though you can use the same via on boards with different numbers of layers. You really only have to create and save a new via if you want to change the drilled hole size or the width of the annulus, and I'm not sure how I'd define a via any other way.

A 'cline' is a complete trace joining two pads together. A 'cline segment' is just one straight line. 'Etch' is anything that ends up copper, including clines, vias, pads, or even text (eg. part numbers or layer ids).

[AndyC_772]

ps. I got a free copy of this book with my copy of OrCAD PCB Designer:

https://www.amazon.co.uk/Complete-Design-Using-Capture-Editor/dp/0750689714

It's a bit out of date now, but still a good introduction to the general terminology and workflow used by the Cadence tools.

[Neilm]

What's up with the via system? Again, I have to have a library of prebuilt vias? What the hell?

Yes, that's how it works, though you can use the same via on boards with different numbers of layers. You really only have to create and save a new via if you want to change the drilled hole size or the width of the annulus, and I'm not sure how I'd define a via any other way.

Keeping vias in a library is very useful. Imagine a company that has the PCBs routed by a sub-contractor. The company may have specific requirements for vias, for instance some use them as test points so they don't need a separate pad or they have them built into pads in some of their footprints to improve EMC characteristics. Passing the sub contractor a library of acceptable vias means the company does not have issues in the future if they need to modify it.

[Alex Eisenhut]

First of all, they're padstacks, this is the basic building block.

You can use a padstack to become a mechanical pin, an electrical pin, a via, or a blind and buried padstack.

Allegro is set up to be used in a structure where people share the same libraries, of course you want the padstacks defined externally and in a library. It becomes VERY MESSY VERY QUICK if you have all kinds of padstacks with wildly different definitions and drill sizes.

An Allegro .brd file is a database that contains not only the layout itself, but all the constraints, symbols, and padstacks for that design.

You can export all this either from Allegro itself or from the command line (system command line, not just Allegro's)

So if you like a footprint you found on someone else's PCB, you can dump it, along with all the padstacks.

Allegro originally didn't have an undo/redo feature. The way it works is you start a command, you are in that mode, as long as you're in that mode you can oops/redo one step at a time, but when you click DONE, you were DONE. No going back!

Allegro now has undo/redo, but it undos/redos the entire command sequence. Like if you route 35 cline segments between two pins, hit DONE, then you want to just undo the last segment and hit UNDO, it will undo the entire 35 cline segments.

But don't worry, once you understand this, it doesn't matter!

If you want to delete just a segment in your cline (the cline being the connect line between two pins, including all the bends), just select edit->delete, or the big X in the toolbar.

Then select all off and Cline Segs in the find filter. If you can't find the "find filter", view->windows->find.

Now you can click on individual segments and delete them.

Now keep in mind, again, you are in the delete mode, once you hit DONE, the undo will undo the entire sequence of deletes you just did.

What if you just want to cut a section of a cline seg? No problem, in the delete mode and cline segs as the find filter, right click your mouse and select CUT from the pop up menu (do this before clicking on the cline segment).

Now pay attention to the command line: it will guide you with terse little comments like "pick first point".

CUT lets you remove a section of a segment between your two clicks.

Also, check youtube, there's a bunch of little 1-2 minute videos showing various commands.

Rotating parts? Super duper easy. Select the part with that four-way arrow thingy, click on the thing (remember the find filter!) and you right click and the options menu pops up.

I don't remember if ctrl-R is default for rotate, but if there is an alias defined for "Rotate" it will appear next to the word "rotate".

If it isn't, go to the Allegro command line, type alias, a space, press ctrl and R, (~R will appear) , a space and type rotate , then enter.

You have now defined ctrl R to be "rotate". So now if you're in the MOVE mode (four way arrow) , ctrl-r puts you in rotate mode.

Here you have many options, like the center point of the rotation, the rotation type, the angle, and how Allegro is supposed to handle connected clines.

Anyways, hope it was clear?

[daqq]

Anyways, hope it was clear?

Thanks, it was!

I knew how to do the rotate thing using the menu, it just seemed a bit clumsy going through a menu to get to it... there is no default keybinding it seems.

Allegro originally didn't have an undo/redo feature.

How does one exist without an undo/redo feature?

I'm kinda getting the how it was meant, but I'm not sure I like it much.

[Alex Eisenhut]

As Jean d'Alembert said, Allez en avant et la foi vous viendra.

push on and faith will catch up with you.
[advice to those who questioned the calculus]

[AndyC_772]

How does one exist without an undo/redo feature?

I first encountered Allegro in 2001 or thereabouts. Back then, not only was it a big, cumbersome beast of a tool, but some of the important features just plain didn't work.

Placement replication was one feature I remember needing, which simply crashed all the time. We were doing (IIRC) a 24 channel board, for which it was potentially a great time saver, but it would crash so often and so unpredictably that we nearly ended up just placing the same thing 24 times rather than use it. We had a regular on-site Cadence rep at the time, and with hindsight, I really feel sorry for him. (To that rep: if you're reading this, please accept my apologies for all the ranting... it was aimed at the product, not you!)

Without undo, you save your work very, very often.

Needless to say, we (the engineers lumbered with actually having to use the software) were unimpressed. A couple of us even got flown halfway round the world to attend a Cadence training course on how to use it, which boiled down to a few days of "here are the non-obvious ways to do things, which have been found not to make Allegro crash".

I left the company not long afterwards, and vowed never to touch it again. But: since then, the bugs have been fixed, and OrCAD PCB Designer has become about the most cost-effective professional level CAD tool out there.

I did the unthinkable: I bought a copy with my own money, which is something I never thought I'd do in a million years.

[Alex Eisenhut]

Ah yes, replication. You have to go into placement edit mode for it to work.

A few years ago I had to replicate 8 high-speed circuits, but I also encountered weirdness. I simply wrote a combo AWK/Excel tool that extracts the coordinates of the components for the master channel, adds a XY offset to the 7 copies, and creates a script for Allegro to run.

Cadence likes to release Allegro early with bugs, you need to install the ISR patches often.