Altium- I am about to cry!! :'( :'( :'( :'( :'( :'(

[chimera_786]

Hello!

So my boss comes in today and says: "here! this is the what I have for you!! Altium Designer 10".. I look at him and say.."what is that?". He shrugs his shoulders and peaces out. As it turns out, its a PCB design software.

So now, along with continuing work on our current product design, I have to learn how to use altium!!

I have been using eagle for some time and im very comfortable with it. Being a design engineer, its expected of me to 'just' know how to work a new PCB software. I have to present this new software in our next design meeting with "positive" results.

I cant seem to figure out even the simple things of this software! Why is designing a custom foot print so hard in this...eh..

I have youtubed and googled.. but nothing is clicking right now between me and this software! Eagle had a tiny learning curve and I was up and working that software when I was in high school. But Altium.. i feel like this should be a course offered at universities to handle this abomination

Where am I going wrong 

[EEVblog]

Altiums "flexibility" in the way it allows you handle and stores libraries can be rather daunting.
But making a new footprint itself is pretty easy.

Here are several videos:



Dave.

[chimera_786]

I did see these videos on youtube. I guess I have no alternative but to learn it..gotta present it in two weeks time.

BTW Dave, I wanted to suggest something to you that came to my mind while I kept up with ur power supply design:

Can you do a tutorial on powering a power supply using a transformer; not a lengthy one--just a 10 15 minute video on choosing a transformer with bridge rectification, smoothing cap (formula etc)---i assume your gonna get much more caught with the whole myth buster deal eh?

The reason why I ask is that because I feel its a very fundamental thing that comes to mind when designing a power supply. I remember when  I designed a power supply, I did not take into account a lot of things i.e in-rush current, PIV rating for Diodes,  using a thermistor to initially limit that in rush current, bypass caps on the primary etc. But later on I did read up on it and tweaked my design but this was a little while ago.

This might help future engineers/hobbyists who want to design a power supply but dont do the necessary research on the dangers of working with mains voltage, transformers, big smoothing caps etc---there are a lot of tutorials that go over using a transformer, LM317s, caps but none of them mention the inherited dangers associated when using transformers and huge caps!

We learn  a lot from your experience and videos. Keep it up!

[Psi]

Altium really is a nice PCB package, and from my perspective very easy to use.
I imagine most of your issues will be created from expecting it to 'behave like eagle'

[Ajahn Lambda]

Agreed.  I found Altium easy to use, powerful (sometimes too much is too much lol), and much more intuitive than EAGLE.  I think once you've messed around with it for a bit, you'll find EAGLE was actually much more painful.


I just wish Altium would get its head out of its ass, and price its product with real-world user needs, much as Dave has said many times.  Well, EAGLE/Cadsoft, too; those are crack prices for such an early-90s-looking product.

[Randall W. Lott]

I almost shat myself when I first used it due to the amount of options.

There are several fantastic YouTube videos on various methods.  I never seemed to have time to make tutorial videos.  You'll likely need to read their web help or watch their videos (which are stupidly only watchable on their site) for more advanced tasks.

Now all other EDA programs seem to be inferior.

[free_electron]

Where am I going wrong 

By trying to use it as you were using eagle.
Different mindset.

If anything is simply in Altium it is making a custom footprint. It has IPc generators, pick your device family , feed it the numbers from the datasheet of the part and voila. you're done. To top it of you go to 3dcontentcentral , find the 3d model download that as a step file in AP214 format. Hit Place - Body , select the step file , click ok hit the number 3 on your keyboard so it switches in 3d view and you place the thing.

One tip , since your boss dropped Altium in your lap : Tell him you ABSOLUTELY need a 3dconnexion spacenavigator. they're like 80$.
This is the bees knees. once you get used to that thing ( pan zoom scroll , rotate , pinch twist , whatever you will be wondering what you were doing with pen-and-paper substitues like eagle ...

Concerning libraries. I always advise people to make a new 'integrated library project' and start pulling in parts from there. You build your library as you go.

a couple of tips. someone sends you an altium project ( schematic and pcb ) you like a certain schematic or pcb symbol. click it to highlight. E -C ( edit - copy )  [ another thing : LEARN the shortcut keys . A sa newbie : keep an eye on the status bar at the bottom of the screen. altium tells you there multiple things in real time : where you are x/y , what you are pointing at ( track and net information) and what it is electricall connected to or what part it belongs to. just hover the mouse arrow over it. when you are in a command it will cycle messages on that bar telling you what you can do tight now. for example : space = rotate , + = layer up - = layer down. These messages cycle every 2 seconds. READ them. in the first 5 minnutes you will pick up what you can do and what the shortcuts are.

But we are wandering off. where was i .. ah yes. you like a symbol. click it hit E C ( edit - copy ) go to your library document ad in the library explorer ( the list with parts in your library ) right-click and select paste. voila. you just 'stole' a schematic symbol. you can do the same with pcb footprints. you can even select mulitple parts at once. hold down shift and click on each one you like. hit E C , go to your library eplxorer , right-clik paste. Boom done.

I have a large Altium library that i maintain. it all compiles into 1 integrated library where everything is linked. including supplier data, 3d models.
P P (Place Part ) 0805R-1k <enter>  boom my 1 kiloohm 0805 is dangling from my mouse cursor.

Another trick : cloning parts. you are placing parts in the schematic. and all of a sudden you need another 100nF capacitor. instead of going back to the parts selector , finding it... simply move your mouse over one that is already in your schematic ( even if there is a resistor dangling off your mouse cursor , just go move the mouse pointer over a cap that is already in the schematic ) hit the INS key (insert) on your keyboard. Presto. altium just 'cloned' whatever was under the mouse cursor and you can now drop that where you needed it. This also works for power objects , net labels etc. You can be placing a net label and switch to a part and back to something else. no need to go dig in menu's . the INs key is your friend.

If you go to the help menu and you type in 'KEYBOARD shortcuts' it gives you a handy page you can print and stick to your wall for the first few days. ( after that you will know the shortcuts )
Shortcuts are easy. Think about what you want to do.
Place Part P P
Place Wire P W
Place Junction
Place Net   P N
Select Inside  S I
Select outside S O
Select All   S A
deselct all is actually X A ( eXclude All )  becasue D A is already in use.

ne need to hold down the <ALT> key like in windows.

most shortcuts are 2 letter, some are three like EMG Edit Move polyGon vertex

pcb editor : + and - cycles layers. if you are routing it will punch a via for you.
page up page down zoom in and out

Later you will create project output and DRC configuration files that are transportable between projects. Altium has excellent free trainaing videos on their site. Accessible from within altium.
Ah , make sure you have a FAST computer ( quadcore with 4 gigs ram)  Altium likes Win7 32 bit the best ( it is NOt compiled for 64 bit since borland is not ready with their compiler yet. It does run on 64 bit but is sometimes flaky). Dual screens with lots of pixels work best. schematic left, PCB right ( or whatever you like )

Another trick : in the PCb editor you can create custom layer views you have one tab per layer. left of that is a box that shows the color of the active layer with a little icon that saya LS on it. click that icon. here you can define your own 'views' ( even with certain items mirrored ) instead of having to mess around with toggling layers on and of depending on what you are ding : create a few custo views ( top layer + multilayer + top silk is on view. bottom layer + bottom silk + multilayer and in MIRROR is another. inner layers can be another view. ) that way you can very quickly switch presets

There is much much more. I have been using this software since it was called Autotrax 1.61 under DOS and came on two 720K floppies. Done every generation. I also use (torMENTOR , Valid, Daisy , Allegro, OrCad, Cadstar , CB5000, EDS (thats to design hybrid circuits)) and have used (P-Cad , Tango , hiwire, Smartwork ( remember that ? )  ultiBoard) and many others . In terms of possibillities, user friendlyness and overall productivity. Can't beat Altium. It's sometimes faster to import an Allegro board in Altium , do the change and push it back to allegro than trying to do it in allegro itself. Or godforbid (tor)MENTOR... speak of the anti-productivity devil... )

If anyone is interested i can post my altium library. It's large.. 53 Megabyte file , so emailing don't work. I'll post it on my webserver and feed a link. And it gets updated almost daily ( i do a lot of designs ... )

[Rufus]

If anyone is interested i can post my altium library. It's large.. 53 Megabyte file

Who doesn't like free

Please PM me a link if you don't want to make it public.

I have also used Protel since it came on floppies (probably 5" ones). I have never had enough experience with other packages to feel competent to praise Altium or criticise its competititors.

[JuKu]

Yes, do learn the keyboard shortcuts. Once you get familiar with those, you want a "game" keyboard, that gives you 20+ programmable keys. It makes a big difference in my productivity to have one hand on the mouse, and one hand has (without moving) single keys for all most used functions.

[westfw]

>> do learn the keyboard shortcuts.
Shudder.  I always figure that "you'll want to use keyboard shortcuts" is synonymous with "the GUI sucks."
Of course, it's a very hard problem to have a GUI structure that is both logical and makes it easy to get to the most frequently used functions.  About the only keyboard shortcut I have defined in EAGLE is alt-Z for "undo", but I make pretty extensive use of the user-defined GUI menus...

[JuKu]

You can use the GUI. It is not the best, but usable. Still, I find it much more faster and fluent to use the keyboard than navigate the GUI. Part of that has to do with the number of things you can do, making the menus big.

[Psi]

Another cool thing,
You can
- Shift select multiple objects,
- Then activate the measure tool (Ctrl-M)
 -And then (while all that is active), use the keyboard Ctrl + arrow keys to move your selected parts around.
One side of the measuring tool will stay anchored to where you set while the other side will move with your selected parts.

This makes it really easy to move parts around until a desired distance is reached.

[hans]

There is much much more. I have been using this software since it was called Autotrax 1.61 under DOS and came on two 720K floppies. Done every generation. I also use (torMENTOR , Valid, Daisy , Allegro, OrCad, Cadstar , CB5000, EDS (thats to design hybrid circuits)) and have used (P-Cad , Tango , hiwire, Smartwork ( remember that ? )  ultiBoard) and many others . In terms of possibillities, user friendlyness and overall productivity. Can't beat Altium. It's sometimes faster to import an Allegro board in Altium , do the change and push it back to allegro than trying to do it in allegro itself. Or godforbid (tor)MENTOR... speak of the anti-productivity devil... )

If anyone is interested i can post my altium library. It's large.. 53 Megabyte file , so emailing don't work. I'll post it on my webserver and feed a link. And it gets updated almost daily ( i do a lot of designs ... )

Agreed, I have tried Ultiboard (done at college, was disguisting to use), then Eagle (I was like, yay we have got better component libraries!) , then got to use Altium once for a few designs and loved it.
I took 2-3 days at my internship to learn it properly, going through their tutorial books. After I got it working I was able to create a novel SMPS + smart dummy load system in under a day, it was so easy and quick to use.
Next intern I had to do eagle.. man it looked so awkward to use. Yeah, if you want to move a component you have to press the move tool. If you want to copy it, you need to press the copy tool. If you want to copy multiple components you have to select the gruop tool, carefully select components, click on the copy tool, right click (left click would ruin your day) and then say 'copy group'. How is that for a convenient user interface design?
In Altium I could just drag my components without changing any stupid 'mode' thing and press CTRL+C. That's a shortcut that almost works in any program, .. text, audio, video, images, and also an EDA. Yay.

Now I am graduating at a company that uses Mentor DxDesigner and PADS. I consider it even more disguisting than Eagle. Like DxDesigner automatically saves a change you make. Undo gets broken from time to time (engineer at company happily told me there is a dedicated button for 'check for system file errors', which fixes the undo option. *pukes*)
If you want to have an old version you are forced to back-up the whole design folder. The design folder consists of tons of directories and files scattered around. How could I grab one schematic sheet out of it and use it in another design? No idea.
Alright, then I just open my old design. "Are you sure you want to close your current project?" What, can't view 2 projects at once? Alright, close my current design and open the other project because I really don't want to be redrawing schematics (chances of mistakes, time, etc.). So I select all components and select copy.
I open my new design, press paste.. Great, it pasted it.. a quirky IMAGE of the schematic. It can't do copy/paste of the schematic itself. I've ran into very similar issues with eagle, it's horrible to use.
In Altium the task of 'copying a piece of schematic' consists of opening the schematic file (which you don't have to close your current design for!), select components (just drag around at schematic), CTRL+C, move to new design tab, CTRL+V, move to position you'd like and click -> job done.

Altium's power is in global management of components and libraries and design reuse (great if you could post libraries vincent! ). The controls of any EDA is different, but as long there is a keyboard shortcut for it's fine. I don't agree that always using keyboards shortcuts is a sign of horrible GUI's. Let's say GUI-only control is horrible because you have to move the mouse all the time.
For example: you're routing your PCB and want to change the trace width. PADS allows you to type W (Width) and then the width of your trace. So W1mm[ENTER] sets it to 1mm. With Altium very similar; press TAB, cursor is on trace width value (and you can edit all other values in this panel as well, like via size if you want to place one etc.), type new value and press enter. You can leave your mouse at the position you left it, so you don't have to carefully reposition it to get the section of trace you already had.
In Eagle or Ultiboard you have to move to dropdown menu's to change the size.. it's so much slower and gets annoying.

The things I mentioned are only the basic tools that are missing from some EDA's, and why I hope you will appreciate Altium sooner or later. I haven't even talked about really useful stuff like routing multiple traces at once (shift select 8 traces on your PCB, click route multiple, and whoila you got 8 lines following your cursor! Press tab to change the clearance between each line, works great) and smart paste in schematic (got a SRAM chip with 19 address pins? Place a net label ADDRESS[0..18], CTRL C, SHIFT+CTRL+V (Smart Paste), Net Label+Wire and select Expand Busses , whoila you got ADDRESS 0 to 18 all labelled on wires you can place in one go at the IC! Quirky symbol that has 18..0 instead of 0..18? Press Y, and all labels get inverted in the Y-orientation. It all makes sense.)

[free_electron]

>> do learn the keyboard shortcuts.
Shudder.  I always figure that "you'll want to use keyboard shortcuts" is synonymous with "the GUI sucks."
Of course, it's a very hard problem to have a GUI structure that is both logical and makes it easy to get to the most frequently used functions.  About the only keyboard shortcut I have defined in EAGLE is alt-Z for "undo", but I make pretty extensive use of the user-defined GUI menus...

NO. let me tell you why.

Altium has a stack based command system. that means you can invoke one commands within commands. There is no way you can do this with a mouse.
lets say you are placing a track. in the middle of the placement you need to move a component. This means you need to abort the placement... ( if you move the mouse the track would follow you all the way to the top screen at which point the vieport begins scrolling. so by the time you have moused over to the menu bar you just messed up your layout... especially when the realtime track push and shove  is on ... )

if you know the keyboard shortcuts you leave the mouse where it is hit M C ( move component ) move the part and when you dropped the part altium automatically returns to the place track mode at the point where you were. This command stack is  fantastic productivity tool.
instead of having to abort an operation, call in something else, go back blabla bla. simply layer your operations.

Besides , having to mouse over to pull down menus is a waste of time. you are concentrating on placing copper and you have to take your eyes off the layout to go find a command. if you know the 2 letter shortcut : bingo.

And get that spacenavigator thing. Spacenavigator left, keyboard middle , right hand on the mouse. You'll be soaring in productivity

@hand : DxDesigner and Pads .. there is a reason i called it tormentor... poor tormented souls that need to use that.

you gave the example of selecting multiple traces and routing them at once. you said shift select. There is an easier way ... Try the S - L shortcut.
you will dray a small line. anything that touchs or crosses the line will be selected.

so , you have a chip with 8 pins next to each other and want to route those 8 pins as a bus. S - L draw a line through the 8 pins and off you go , There is also S -U ( inside a rectangle you draw )

[Randall W. Lott]

Give it a few days of disciplined learning.  It'll become easy.

This is coming from someone who finds Eagle confusing.

[baljemmett]

The controls of any EDA is different, but as long there is a keyboard shortcut for it's fine. I don't agree that always using keyboards shortcuts is a sign of horrible GUI's. Let's say GUI-only control is horrible because you have to move the mouse all the time.

It's actually all orthogonal -- command set and interaction style are two different facets of UI design, and looking at them in isolation can lead to trouble.  For instance:

For example: you're routing your PCB and want to change the trace width. PADS allows you to type W (Width) and then the width of your trace. So W1mm[ENTER] sets it to 1mm. With Altium very similar; press TAB, cursor is on trace width value (and you can edit all other values in this panel as well, like via size if you want to place one etc.), type new value and press enter. You can leave your mouse at the position you left it, so you don't have to carefully reposition it to get the section of trace you already had.
In Eagle or Ultiboard you have to move to dropdown menu's to change the size.. it's so much slower and gets annoying.

In Eagle, you can just type the new width during routing and it's applied.  I believe that's because Eagle is actually driven by a command line, and all the 'tools' you can choose are basically just macros to enter the equivalent command.  So to route a signal called FOO with a 10mil trace you could click the route tool, select 10mil in the dropdown, click the FOO airwire and route it -- or you could type ROUTE FOO 10mil, or ROUTE 10mil FOO -- or any combination of the above (e.g. click the tool, then just type signal names and/or widths as you go.)

I know it's just an example, but it goes to show that understanding how the command model works for a package goes a long way towards influencing how logical it seems to use it.  They all have strengths and weaknesses, and what one person finds great (like keyboard shortcuts) others will hate.

[chimera_786]

off topic.. but this is why I absolutely love this forum!!! Every one here bothers to chip in with ideas and questions. I am a member of several forums..but this one has proven to be the best!!

Thanks for the input guys..btw..my boss did ask how Altium was working out.. all I did was: shrugged and gave a thumbs up. That is SO NOT THE CASE!!!!!

It is a very extensive software and I feel that I need better documentation becaz of just the shear number of options! I dont know why but up till now, I feel eagle is my staple PCB layout software. I am trying hard to break the chains and learn altium..its just a painstaking task becaz I cant do it at work due to other engagements and I cant do it at home caz well..im tired!!

So only this weekend will I be able to go to town on Altium, hopefully!

[free_electron]

you can not compare tools like Altium, CB5000, DxDesigner and others to Eagle, Kicad, Diptrace and others. They are in a different league.

To give you an idea of things you can do with altium ( And these are things i have done... )

I make a schematic. This has some analog stuff, some digital stuff and an FPGA. I wirte some verilog code in altium that ends up in the FPGA. I instantiate a CPU from the ip library that comes royalty free with altium in the same FPGA. I write some C code for that cpu (altium designers has the C compilers built in for all the cores..)

I do simulations on the analog block using the built in simulator. I do the same for my verilog code.

When i'm confident my hardware portion is ok i push the whole shebang to the pcb , import a 3d model of the case it needs to end in, do the parts placement ( including full 3d checking so i know it will fit.), make the memory interface using automatically tuned length equalisation and do some controlled impedance calculations. Pin swaps on the FPGA directly propagate in my code.

When the board comes in, i assemble it and connect it to Altium using the little JTAG adapter (150$) they have.  From within altium i now compile the cpu's source and the fpga , download it into my board. And here is the kicker : If i push one of the buttons on my board , attached to the fpga , the trace in the PCB viewer changes color to reflect the logic state. I can click on a pin of the fpga in the PCB viewer and tell it to turn this pin high or low. I can set breakpoints in my c code. When i push a button on my pcb the code editor neatly breaks at that position.

I don't need ANY other tool than altium. Everything is done inside this one project. Everything is tied together. I don't need to learn 25 different tools and user interfaces or fidget around trying to import files between tools, or do extra effort making sure everything aligns between all the different tools.

All i need is my Altium installation ( and the free versons of Xilinx , Altera , Lattice and other FPGA compilers . Altium talks to these in the background. I don't even have to open those or learn how to use them). For 5K$ ... it's going to be EXTREMELY hard to beat that.

Now, take a look at what your current design tool' can do and then pull your conclusion... Are you in the 'design tool' category or in the 'pen-and-paper replacement' category...

If you're still not convinced... you kow those two little rovers on mars that have been bravely soldiering on for 5 years or more and sending us all these great pictures of the red planet ? Guess what...
All the boards in them were made on Altium... I don't need more convincing than that... ( of course it's the brilliant humans that sat behind the screen that need to get the credit for the design. But the fact they chose Altium... that say's enough )

PS. I am NOT affiliated with altium ! Just a VERY happy user ( i even bough my own licence for hobby use. A couple of years ago they had a deal for 2500$ and i bit the bullet then. It was that or a new video camera...) .

I do about 20 projects a year (at work) and this thing has never let me down. Yes, it does have its odds and ends and quircks. ( and sometimes locks up, but that is solvable by having a GOOD , CLEAN machine ) And it has a long learning curve. But it is incredibly flexible and powerful. You can create your own scripts , create project templates , tie it in to purchasing , backend processing , documentation output. I even pull in designs from other tools ( PADS , Zuken ) , or import gerber and decompile that into PCB data so i can make sure my part of the design will fit. I've done test socket desing for very complex packages and modeled the entire thing in Altium. Export step file , import step in soldiworks and transfer it to the mechanical department. When they are done 'massaging' the design i pull it back in and verify it still fits the footprint. And yes altium has shortcomings too.. EMC and field solving is not possible, but, it integrates seamlessly with CST studio and Hyperlinx. So there is your solution for that. this thing is an Electronics Design tool. Not just a 'schematic capture and pcb drawing tool...

[Rufus]

you can not compare tools like Altium, CB5000, DxDesigner and others to Eagle, Kicad, Diptrace and others.

You can if all you actually want to do is schematic capture and PCB layout which is what the majority of their customers really use it for.

The analog simulator is pretty much junk, it just doesn't have a good spice engine.

The FPGA stuff is done quite well and is a product of Altium's vision of one day all electronic designs being a systems built on FPGAs and a development tool that did the whole job would sell like hot cakes.

That vision was flawed, it hasn't happened and won't because dedicated silicon has progressed as fast or faster than FPGAs so an FPGA based system for the sake of it or because you can is hardly ever the right solution. When you really do need an FPGA you have to put up with being a generation out of date because Altium support lags behind the vendors.

So the FPGA and embedded stuff is nice but mostly useless. The reason it is bundled with schematic capture and PCB is if it was a realistically costed optional package hardly anyone would buy it.

More recently they have been wasting money on their next flawed vision of the future of everything being in the cloud and the idea of selling EDA 'apps' and IP like iTunes sells music. Their vision also included all future electronic designs being part of an 'internet of things talking to the cloud'.

It has gone very quiet on the 'internet of things' bit, possibly because it is a junk idea but more likely they don't have any people or money to work on it. Perhaps they are beavering away at it in secret which means my subscription is buying more junk I don't want. They are still spending their time dicking around with Altium Live and the cloud with the occasional scrap of bug fix and improvement to the core tools to try to keep the people who are paying for it all happy.

I think you are the first Altium "VERY happy user" I have come across. That said I haven't come across many that think they would be happier with something else.

[free_electron]

You can if all you actually want to do is schematic capture and PCB layout which is what the majority of their customers really use it for.

Then you don't need Altium. Agreed. although , it is still a really good Schematic / PCB tool.

dedicated silicon has progressed as fast or faster than FPGAs

That has always been the case. But 99.9% of the electronics engineers out there have no access to a silicon fab.. Need something custom ? FPGA is your only option... And for those people that have access to a silicon fab ( like me) : we still use FPGA to prototype blocks before we spin the first wafer. At a cost of about 1.3 million $ per mask these days ... you do run your system on a FPGA first...

being a generation out of date because Altium support lags behind the vendors.

No it doesn't. All you need to do is keep your Quartus / ISE or other FPGA software up to date. Altium uses only the backend bitstream compiler and the route rin those tools. If altera ( i use mainly Altera ) releases new devices they also release a new version of quartus. Simply install it and done. You can immediately use it in Altium.

idea of selling EDA 'apps'

  you got Altium and OrCrap confused. Cadence is the 'OrCad now does Apps' too' maker.

I think you are the first Altium "VERY happy user" I have come across.

You must not have met many Altium users then. I don't know where you are located, but here in 'the valley' there is the Altium Users group. We meet a few times a year ( Last couple of times was at National Semiconductor and Tesla Motors. Altium presents a few features and does mini trainings during these meetups , after which real users ( typically from the company hosting the event ) present how they use certain features of the tool and share their 'tips and tricks'. Very educational. ( and there's free food and a raffle as well ). Draws a bunch of people and they're all happy people. Yeah , there's the usual friendly fire about 'havent you guys fixed bug xyz yet'. But that is the cae in any of these user groups. Visit a synopsys users group and it happens there also. Visit a linux users group and it is all out thermonuclear warfare ... ( vi vs emacs and gnome vs kde or whatever distro today is the 'hottest' ). comes with the territory.

[Rufus]

dedicated silicon has progressed as fast or faster than FPGAs

That has always been the case. But 99.9% of the electronics engineers out there have no access to a silicon fab.. Need something custom ? FPGA is your only option...

The large majority of electronic designs don't need something custom because there are 100 semiconductor manufacturers out there trying very hard to make dedicated silicon solutions for all requirements. Altium thought FPGAs were going to get so cheap it wouldn't be worth using dedicated silicon but dedicated silicon got cheaper and more capable even faster and continues to need less power and support circuitry.

Even when you do need an FPGA for something custom the choice of using a small FPGA and sticking  for example a cheap ARM outside it or a larger FPGA with embedded soft core isn't straightforward.

So like I said the whole system on an FPGA end to end design solution Altium provides is more or less useless because whole system on FPGA designs are more or less useless.

being a generation out of date because Altium support lags behind the vendors.

No it doesn't. All you need to do is keep your Quartus / ISE or other FPGA software up to date. Altium uses only the backend bitstream compiler and the route rin those tools. If altera ( i use mainly Altera ) releases new devices they also release a new version of quartus. Simply install it and done. You can immediately use it in Altium.

If that were the case why does Altium need to install about 1GB of device family specific hardware support files which includes things like Spartan 3AN specific DLLs?

idea of selling EDA 'apps'

  you got Altium and OrCrap confused. Cadence is the 'OrCad now does Apps' too' maker.

You haven't seen the Altium Content Store where currently (and farcically) everything is free?

[EEVblog]

you can not compare tools like Altium, CB5000, DxDesigner and others to Eagle, Kicad, Diptrace and others. They are in a different league.

To give you an idea of things you can do with altium ( And these are things i have done... )

Yes, it can do all that stuff, in theory, but in practice you would be one of the few people who use it to it's full extent like that.
Simply because Altium cannot support all FPGA's for example, or really high spec high speed design, and once you need to step outside the limited comfort zone of what Altum supports in those areas, then you are left holding an empty bag.
More than 95% of Altium users simply use it as an advanced PCB and SCH tool, like they always have. Many of those don't use it for anything else because they are afraid it's going to let them down in the non-PCB areas when they need it the most.
But yes, some of the integrated stuff it can do is very cool, and it's quite attractively price in it's niche. The lack of competition at the price point is what has kept Altium going.

Dave.

[EEVblog]

You can if all you actually want to do is schematic capture and PCB layout which is what the majority of their customers really use it for.

It's more than a majority, around 95% is my educated guestimate.

The analog simulator is pretty much junk, it just doesn't have a good spice engine.

Yep, and it clearly hasn't had any significant work done on it in years.
Similar with the signal integrity and the autorouter, although SI seems like it might be getting some attention now.

More recently they have been wasting money on their next flawed vision of the future of everything being in the cloud and the idea of selling EDA 'apps' and IP like iTunes sells music. Their vision also included all future electronic designs being part of an 'internet of things talking to the cloud'.

Yeah, shame it will only apply to a very small percentage of the PCB/SCH CAD market, and just like FPGA's, they don't have the resources to make it universally usable. You can bet the farm that this vision will fail, and fail dismally.

It has gone very quiet on the 'internet of things' bit, possibly because it is a junk idea but more likely they don't have any people or money to work on it. Perhaps they are beavering away at it in secret which means my subscription is buying more junk I don't want. They are still spending their time dicking around with Altium Live and the cloud with the occasional scrap of bug fix and improvement to the core tools to try to keep the people who are paying for it all happy.

They appear to be spending much of their effort on the core tool recently, because if you read the Altium forum, it's all that the users are screaming for. They don't care about the vault, the cloud, or the internet of things. So they are at least listening again.

I think you are the first Altium "VERY happy user" I have come across. That said I haven't come across many that think they would be happier with something else.

And that's the only reason Altium have gotten away with going off the deep end over the last decade or so, in pursuit of their silly visions.
The loyal core PCB/SCH user base sticks with them.

Dave.

[free_electron]

The large majority of electronic designs don't need something custom because there are 100 semiconductor manufacturers out there trying very hard to make dedicated silicon solutions for all requirements.

yes, agreed, but .. for every 100 problems these 'standard' things solve there are 1000 problems the standard stuff does not solve..
Want proof ? Xilinx and Altera are still shifting a truckload of their parts. If everything was solvable with off-the-shelf parts they would have long gone out of business. Many 3D TV's and large format LCD's have an fpga on board. Open the new Fluke bench multimeter ( the one that is also sold under tektronix name ). It's got two altera's in it. The in-guard has the multislope engine on board and communicates over an optical link to the outguard. that one has a nios engine and runs linux ( that's why that stupid meter has a 20 second boot time if you do a cold start. )

FPGA's DO have their place and ARE actively used. there is a 'band' where the cost picture to switch from 'off the shelf' to 'full-custom' is not feasible. Custom has a very hefty price tag and long design cycle. plus its not flexible if you want to 'update on the fly' your time-to market is too long. That's where FPGA's step in. The risk is much much lower, even though the chip itself costs more.

Altium thought

i'm not going to speculate what altium thinks, its none of my business , or interest. point is that, if you are doing end-to-end design (schematic , analog , pcb , fpga ,cpu ) they provide you with a single tool. I like that ( that doesn't mean you have to agree with me. There's tons of people out there that like to spend days making TCL script and other widgets to glue different tools together. Me ? not interested. Fastest , least effort path is well enough, I'll use the free time to go scuba diving  or tinker with my own 'pet projects'.

Even when you do need an FPGA for something custom the choice of using a small FPGA and sticking  for example a cheap ARM outside it or a larger FPGA with embedded soft core isn't straightforward.

Funny that you should mention that. that is exactly what i did a couple of years ago. I have a board with an ARM7 mapped into a Cyclone 2F50. A cypress FX-2 USB processor is also mapped into the FPGA and allows me to down load the bitstream and interface the PC with the guts of the system. I'm not going to bore you with the architecture, or what it is for, point is this rickety little ARM7 at 48MHz runs circles around a dual core ARM9 screaming at 800MHz that sits in a -VERY- expensive asic. Simply because i don't have to waste cpu cycles on complex things. If i find out the cpu is too heavily loaded for a particular task i simply change it from a software routine to a hardware co-processor that i plunk in the FGPA.

system on FPGA designs are more or less useless.

I agree on that. 'system on fpga' is useless. But System 'with' an FPGA is extremely powerful. Take off-the-shelf SOC, glue an FPGA on and off you go.

If that were the case why does Altium need to install about 1GB of device family specific hardware support files which includes things like Spartan 3AN specific DLLs?

because those contain the backend compilers. Altium does NOT perform any place and route. It has a code editor , that tie into the schematic and PCB , a debugger , but for everything else they simply talk to the xilinx tools. And that is good. altium doesn't spend time on developing an FPGA tool. they provide the 'glue between the FPGA tool , my board my schematic and they give me a nice debug environment to work in (push button on board , trace highlights on layout and vice versa. This shortens my time to bring up the board for the first time tremendously. ) That, and i don't have to learn another user interface if i switch FPGA ( altium doesn't care if you use altera, xilinx, lattice , actel or whatever. No need to learn new tools)

You haven't seen the Altium Content Store where currently (and farcically) everything is free?

yes i have. They don't call them 'Apps'. OrCad officially call them APPS. I was at Designcon West last week and Cadence had a big banner over their booth. 'OrCad does Apps Too'. and most of them are 'paying' apps.

Now, this 'simulator is pretty much junk'. I don't see any difference between what i run through Eldo (now that's a simulator !)  or Altium.. OK altium is slower and there's things it doesn't know how to do. If you feed it the right models it does as good a job as any other spice simulator. Besides... simulator output should not be trusted until the design is actually built and has been verified on bench. Tuning an opamp filter works just as well in altium as it does in any other simulator. And i don;t have to redraw the schematic in a foreign tool and then draw it again in the pcb tool. Saves me time.

Then again , 80% of what i do is digital. I  have only used the sim to tune analog filters. Anything beyond that is done on bench.

[Rufus]

yes, agreed, but .. for every 100 problems these 'standard' things solve there are 1000 problems the standard stuff does not solve..
Want proof ? Xilinx and Altera are still shifting a truckload of their parts.

Xilinx accounts for less that 1% of the semiconductor market by value. Altera is smaller.

Altium thought

i'm not going to speculate what altium thinks, its none of my business , or interest. point is that, if you are doing end-to-end design (schematic , analog , pcb , fpga ,cpu ) they provide you with a single tool.

That isn't the point, we know it does that (with limitations) the point is how many people are doing end-to-end design (schematic , analog , pcb , fpga ,cpu ) and especially how many of the Altium users who are currently paying for it. Like Dave says it is probably around 1 in 20.

If that were the case why does Altium need to install about 1GB of device family specific hardware support files which includes things like Spartan 3AN specific DLLs?

because those contain the backend compilers.

And you can't design in a part without a back end compiler (etc) and Altium lags behind vendors providing that compiler (etc) for new parts so if you want to use Altium for your FPGA flow you have to settle for being a generation out of date. It isn't as you claimed a just a matter of keeping your vendor tools up to date, doing that doesn't help and potentially breaks Altium. It currently only officially supports ISE 12.1 not the current ISE 13.3 for example.

You haven't seen the Altium Content Store where currently (and farcically) everything is free?

yes i have. They don't call them 'Apps'. OrCad officially call them APPS. I was at Designcon West last week and Cadence had a big banner over their booth. 'OrCad does Apps Too'. and most of them are 'paying' apps.

Call them apps, call them plugins who cares.

Now, this 'simulator is pretty much junk'. I don't see any difference between what i run

Then you can't have used it much. It failed to simulate about half the circuits I ever tried. At times I dragged and dropped the .nsx netlist onto LTSpice to let it (instantly) converge on a operating point then plaster the Altium schematic with .ICs and values copied from LTSpice just to get it to start a transient simulation. I don't know if it is actually bugged or just lacks engine tweaks and optimisations which even free packages like LTSpice have. I don't bother any more and just use LTSpice in the first place now.