DEX eval by free_electron

[free_electron]

Nobody else does this...

i've seen multiple .net based programs doing that ... they look for binding and run the JIT once upon installation to create the final links. .NET relies heavily on JIT. by doing this step at install you avoid to have to run the JIT every time at startup. run it once at install and save the binary. this saves startup time and runtime as well.

that is probably what he is doing.

[Wilksey]

Holy shitballs!

That's a lot of experience!

[free_electron]

anyway. after this stuff , back to the review.

while waiting to find out how to turn the darned autowiring off i decided to go and start a blank project and see if i can manage to find me some parts and place them.

creating new project is easy. 
parts browser is well organized 

however, the first part i found is a big problem ...
capacitor  C?
footprint : U?

ehh .... that can't be right

[free_electron]

ouch ...
Passive - Capacitors - Chip - capacitor ...

ehhh ...  really ?i may be wrong here , but something says me that ain't quite right .... chip capacitors don't have such a footprint and they ain't called U ...

this is not good ...

[free_electron]

ok , now i am getting slightly pissed ...

do you even know the difference between an electrolytic and a chip capacitor ? do you know that U is used for integrated circuits and X is reserved for crystals ?

and there is no way in hell that 0805 can hold 440 volts ac either ....

The classification is nice but folders are empty ( community is completely empty. it has some names in it but all empty) and what little is there has wrong footprint assignments .

Are there libraries somewhere i can start from ? i don't really want to make a whole bunch before i can draw anything...

[nctnico]

Nobody else does this...

He probably refers to the .NET libraries compiling themselves and probably generating new bytecode for the .NET software he wrote. Due to the inherent overhead the advantage is probably insignificant.

@Free_electron: I'm waiting for you to get to the part where you create a bill-of-materials...

[free_electron]

ok. i'm now trying to create a part ...

first off : why is everything automatically called 'U' if i pick a resistor, capacitor , transistotr diode .. it's all 'U' 
Second : there are some SERIOUS bugs in the part generator ...

click on the resistor. then click on the bottom left block capacitor. you get a funny 4 terminal capacitor ?
now click on the bga picture and click back on the block capacitor you get a 64 pin DIP component this time ...

that isn't quite right ....

[free_electron]

it is getting worse and worse.
i try making a simple capacitor.
trying to move the white border has the screen start 'shivering'.  The viewport jumps all over the place.

- Moving a pad resizes the white border as well. wtf ?
- i can't even move the pads back to their original position as they are off-grid now.
- there is no way to change the grid spacing.
- there is no coordinate view. i cannot select a pad and type in for example 2,0 to have this sit at 2mm to the right of the zero origin. you have to do everything 'by eye'
- there is no way to enter coordinates for elements.
- what if i need two pads to be 4.3 mm apart ? or 0.65mm ? how do i do that ?
- how do i resize pads , change shape ?
- how do i draw the outline ? put a text string on it ? put other artwork on it ?

and clicking next really eats the cake... i selected a CAPACITOR !!! why the hell do i get a resistor symbol
how do i edit this symbol ? i can only move it as a group. i can't even figure out how to draw a capacitor symbol in it ? it's just a rectangle labeled U with two pins ( can i at least see the pin numbers so i know what pin on the symbol corresponds with what pad ? i'm trying to make a polarized cap ...



i just tried to make a BGA. where do i even type in how many rows and columns this thing has ? what about ring cutouts ?
Your BGA pin numbering is incorrect too ! It is not allowed to use I, O, Q, S, X and Z in the pin numbering of a BGA  ! There are STANDARD to be followed !

Dare i say it ? ... yes i will was it : this is one more cad program made by programmers that have no clue what the rules are or how it will be used. you might as well have this thing use a grid set in fractions of a furlong and annotate surface as the number of cows you can fit on it.

- using the scroll wheel to zoom in the footprint view does not work. how the hell do i zoom in ? i need to right click and go click zoom in every time.
- the scroll bars work but the arrows on the scroll bars do not work ? the scroll bar moves when clicking the arrows but the viewport doesn't move ?
- for some reason suddenly scroll wheel started working. don't know why.
- if i click in an empty space on the window ( like left of the '<back' button ) a help window opens ? if i close the help window now scroll wheel zoom doesn't work anymore. even clicking the window top bar ( to get focus to the window ) does not restore it.

i'm sorry to say this but your part editor is complete crap ! it is full of bugs, the footprints it generates are wrong , and the symbols are wrong.

[Iliya]

You forgot to tell everyone they can download AutoTRAX from:

http:://pcb.software

and judge for themselves or follow along with your steps by step critique. http://en.wikipedia.org/wiki/Critique

[nctnico]

@Iliya:
Free_electron isn't the most forgiving person when testing but he is thourough so take note of his problems!

A side note:
One of the things I like about Orcad layout is that you can input pad locations in a spreadsheet. It saves a lot of grief from having to use the mouse to position a pad. Nowadays many SMT parts need pads at odd coordinates like X=1.233, Y=8.911. With a spreadsheet you just punch in the numbers. Same for placing components later on. I have designed several circular LED boards for a customer. I wrote a small program which can calculate the position and rotation of the LEDs and Orcad Layout allows me to type those numbers into a spreadsheet view with the component locations.

[Iliya]

ok , now i am getting slightly pissed ...
Are there libraries somewhere i can start from ? i don't really want to make a whole bunch before i can draw anything...

Eagle Parts converted. Don't blame me! I would NEVER use a library part. Check, Check and check again.
http://pcb.software/Download/Parts


Then perhaps AutoTRAX is really not for you and Altium is more to your liking. Don’t know why you are doing this. (Well I do really) Is it because I posted on the ‘free Alltium is coming’ topic (but it’s not coming) or is it because it’s a threat.  Must really hurt.
AutoTRAX is NOT Altium Designer. It never will be. It will be better and far, far cheaper.
Nick-picking on a library fault! Never trust libraries, 100,000 part libraries – how many faults in them! Just change the U to a C or even to Cap.
I am prepared to help you with your troubles, but this really is not the way to do it. Seems you want a bun fight.  I do not.
So please do this review correctly and objectively, not just darting about picking for issues. Go and spend some time with the software, resolve your problems, watch a few videos, there are 92, HD videos, (Set up your player to HD) and then come back. Remember, AutoTRAX is not Altium it’s better.
Remember, you might have a vocal group of Altium followers, but there are far more onlookers. Look at top of the topic to see who’s looking.
Can you please point us to where you did a similar review say of Altium?
P.S.  Try exploring the menu and you will see buttons like Shortcuts, yes there is a shortcut editor.

[free_electron]

@Iliya:
Free_electron isn't the most forgiving person when testing but he is thourough so take note of his problems!

no i am not i expect stuff to work and to be correct ! imagine doing a board with that bga numbering to be wrong ! that is a disaster !

that being said. i suspect there is something i don't know going on.
i get the gut feeling that this library wizard is only a 'linking' tool and that the actual creation of the symbols and footprints is done elsewhere in the program.
i'm gonna prepare dinner now and watch some of the video's later tonight. there is something i am missing. i still have hope for this thing .

in any case : this program has a bunch of quirks and some serious bugs ( getting the BGA pin numbering wrong is unforgivable ! ).
also , you really need a generator for things like qfp where i can typ in the pad size and shape , the pitch , the span of the part, the boady span and it generates the footprint.

we also need a numerical coordinate view and editing .so that i can click a pad and type in the width and length and its x and y position. creating footprint 'by eye' is not done ! they need to be exact. i also need a way to edit solder mask opening over a pad so i can encroach or use SMDP. same for paste mask opening. i need to be able to create custom openings for the paste mask. Thermal pads in tqfp typcially need to be shrunk while the pins need overprinting and a lattice needs ot be constructed in case there are thermal via's.

I may be wrong but my gut feeling says that Ilyia has never really made a 'real' PCB beyond maybe some simple stuff with thru hole components.

there are other problems in this thing. for example if i pick a vertical resistor : there needs to be an indicator where the body needs to be placed ! typically such parts are places with bodies alternating left and right so i need to see this in the pcb footprint.
also , body diameter can change . so can pitch.

[free_electron]

Eagle Parts converted. Don't blame me! I would NEVER use a library part. Check, Check and check again.

wait ? you STOLE some other CAD programs parts ? And you are going to point fingers at that other cad program now ?

because it’s a threat. 

bwahaaaaa

It will be better and far, far cheaper.

cheaper, definately no argument there. better ? maybe in 10 years ...

look i've said this before : i am trying to give you some brutally honest pointers on what a good schematic pcb cad program needs to provide to its users.
i am exploring this thing and running into several problems. some of these are problems on my side because i am learning this program. some are 'taste' problems .
but some are problems that you as a program designer need to take into account ( like colorblind people !) UI design is extremely important for accessibility.

Your default symbol library is junk. symbols linking to wrong footprints. i spot these things because i know what it is supposed to be. imagine for a second a new guy that wants to make his first board. he picks a few parts and makes the board and NOTHING but NOTHING fits on the damn board because what you provide ( don't point at eagle and tell me it's their fault. that is not an excuse. you shouldn't have used that to begin with. besides, it's not yours. i'm sure the eagle guys won't be too please it they find out you stole their libs ... ) is wrong.

at least provide a minimal library with a few resistors, caps and ic that is correct. how can anyone even begine making a board with this. especially for new people trying to make their first board. they can't trust anything !

I am prepared to help you with your troubles, but this really is not the way to do it. Seems you want a bun fight.  I do not.

it ain't a bun fight ! i gave a whole bunch of points i like. i also gave a whole bunch of point's i don't like.
i give you the opportunity to learn from someone who has done a bunch of boards in his life and knows the rules. use it to make your program better !

as for helping : you can begin by telling me how to turn autowire off in the schematic.

So please do this review correctly and objectively, not just darting about picking for issues. Go and spend some time with the software, resolve your problems, watch a few videos,

i will watch some tonight especially on parts creation. i'm hungry now. more tomorrow

Remember, AutoTRAX is not Altium it’s better.

i guess companies like Siemens , BMW , NASA, Nokia, Microsoft, Volkswagen , Seagate , Linn , Boeing . Airbus and thousands of others must be wrong because they use inferior Altium instead of your Autotrax ...   

And you say i have an attitude problem ? pot <->  kettle.

Weren't you the one that stated in the Altium topic that you needed some users ?
Unfortunately now you found one you may not be able to handle ...

[Iliya]

@Iliya:
Free_electron isn't the most forgiving person when testing but he is thourough so take note of his problems!

no i am not i expect stuff to work and to be correct ! imagine doing a board with that bga numbering to be wrong ! that is a disaster !

that being said. i suspect there is something i don't know going on.
i get the gut feeling that this library wizard is only a 'linking' tool and that the actual creation of the symbols and footprints is done elsewhere in the program.
i'm gonna prepare dinner now and watch some of the video's later tonight. there is something i am missing. i still have hope for this thing .

in any case : this program has a bunch of quirks and some serious bugs ( getting the BGA pin numbering wrong is unforgivable ! ).
also , you really need a generator for things like qfp where i can typ in the pad size and shape , the pitch , the span of the part, the boady span and it generates the footprint.

we also need a numerical coordinate view and editing .so that i can click a pad and type in the width and length and its x and y position. creating footprint 'by eye' is not done ! they need to be exact. i also need a way to edit solder mask opening over a pad so i can encroach or use SMDP. same for paste mask opening. i need to be able to create custom openings for the paste mask. Thermal pads in tqfp typcially need to be shrunk while the pins need overprinting and a lattice needs ot be constructed in case there are thermal via's.

I may be wrong but my gut feeling says that Ilyia has never really made a 'real' PCB beyond maybe some simple stuff with thru hole components.

there are other problems in this thing. for example if i pick a vertical resistor : there needs to be an indicator where the body needs to be placed ! typically such parts are places with bodies alternating left and right so i need to see this in the pcb footprint.
also , body diameter can change . so can pitch.

I worked for Ferranti Electronics designing and building SMPSs.
GEC as head of Research, on car multiplex systems. Yes 2 papers at IEE in London.
I have only 1 patent to my name assigned to Cardiff Software.
I don't write books or give my code away.
I have a honours degrees in Physics from Birmingham University and did my Ph.D studies in 3D user interfaces at Wolverhampton University.
Worked at Motorola and National Semiconductors on photolith process and development.
Yes I have designed many PCBs, years ago, including using tape X4 on clear film. Ferranti/GEC.

I think you need to slow down,and think before you write. Spend some time reviewing the menu, videos etc.
I bet nobody starts up Altium and within 4 hours has their completed PCB!

[c4757p]

Eagle Parts converted. Don't blame me! I would NEVER use a library part. Check, Check and check again.

wait ? you STOLE some other CAD programs parts ? And you are going to point fingers at that other cad program now ?

Oh, dear.

[Iliya]

Weren't you the one that stated in the Altium topic that you needed some users ?
Unfortunately now you found one you may not be able to handle ...

I said users in the constructive sense. I have serious doubts about your review. It appears to be an Altium user with Altium preconceptions having a go.
Please conduct a rational review rather than darting about picking problem.

[miguelvp]

Weren't you the one that stated in the Altium topic that you needed some users ?
Unfortunately now you found one you may not be able to handle ...

I said users in the constructive sense. I have serious doubts about your review. It appears to be an Altium user with Altium preconceptions having a go.
Please conduct a rational review rather than darting about picking problem.

I'm not an Altium user and I don't see his review to be irrational, he is pointing out problems that you can correct, you should look at this as valuable feedback instead of thinking it's an attack, he is doing you a favor believe it or not.

[free_electron]

i just figured out that that footprints are stored as a.part file.
apparently you are not supposed to muck about with them in that library editor ( why on earth can you manipulate part elements there then ! if you are going to allow manipulation there make it complete )

i loaded that capacitor part to try to fix it. clicking the 'properties' button on the menu. doesn't do anything. clicking it one more time gives me this : 'please restart' (image 1)

prior to that i noticed a couple of things in the editor. you treat the objects as you would make a vector drawing program. for example i can make an oval shaped pad. (simply warping a circle to an oval.) you can't do that !

i placed such a part on the pcb ( with an oval pad) then generated gerber and DEX completely froze.

When i try to launch DEX the windows menu link is broken. ' the program has been changed or moved' ... right clicking and selecting properties shows that your try to run Autotrax.exe as opposed to dex.exe ... looks like your installer needs some work too.

imagine me now muttering something like " better than altium ... right ...    he can't even get the link on the windows menu right. "

now. i have tried to generate gerber from this simple single component. ( a single capacitor with one round pad and one oval pad. )
your gerber generation is wrong.. i also do not like this 'all blalbla will be blabla. the gebrer should be EXACT to what is drawn on the board. you can not start altering layout primitives by adding endcaps. if there are endcaps i need ot see the m in the pcb view. gerber shapes need to math pcb shapes 100% !

Gerber problems  : first of all the oval pad is not generated as a flash (it doesn't have a d-code). that means the pcb fab cannot detect this as a pad and they cannot do connectivity test on this as they go by flashes and not by strokes. afaik gerber has no provision for oval pads to begin with ... so you should not allow that to happen.

Your text renders completely wrong. it creates garbage all over the plots. you are not closing the end stroke. (see third image : C1 connects with a stroke to the 'non commercial' string. you forget to send the correct code there.

These are serious problems as it makes the board unmanufacturable. There is nothing wrong with the design. the output is wrong.
i will try to open this on monday using FrontLine and see where the problem really sits so i can tell you what to fix in the gerber generation. ( Frontline can trace gerber files line by line so i can see at exactly what step the line appears and what D or G code is missing.


-edit- i looked at it with Zofz and your fonts is completely rendered wrong , including the part designators. this needs work as the gerber output is unusable.

[free_electron]

to summarize today :

The good
- it starts quick and reacts quickly to operations part due to the JIT launching once at install.
- supports multi monitors
- the UI is relatively uncluttered

The bad
- the installer creates a shortcut to 'autotrax.exe as opposed to dex.exe and autotrax.exe does not exist ...
- window minimizing maximimizing is wonky on dual screens.
- scroll wheel  zoom/ pan is 'abnormal' ( not like most programs)
- autowiring is a royal pain in the ass and makes spaghetti of the schematic and creates shorts.
- no parts libaries and whatever is there is not right
- parts generation is wrong. caps show up as resistors, footprints are wrong ,standards aren't being followed.
- gerber output is wrong

the wishlist
- space navigator support. any cad program medio 2015 not supporting a spacenavigator is just ... a toy.
- Menu's should move with the window. if i have schematic on the left monitor and a pcb on the right monitor the schematic menu's should be there where they belong. now everything is on the 'main monitor' sou you have to mouse over the screens to get where you need to be.

Please do not see any of this as an 'attack' and do not take it personal. As a seasoned pcb designer i am torturing this tool to see if this is usable. The things i find are things that should not be there ( i have found several other things i am not mentioning here because they fall under 'personal taste' )

The things i do flag here are problematic and need fixing. it is inexcusable to go 'i copied eagles library'. your default library is very empty. Right now for the design i want to do i have to create all parts. there isn't even something as simple as a 1K resistor in that library. that is pretty poor.  i'm deliberately not ranting about it not being able to link to digikey / mouser/ avnet/ rs websites like the big boys such as altium, mentor and cadence do because i know that you don't stand a chance tapping into that system. that is out of your league . for this review it is irellevant. i am reviewing base functionality and usage.

my review is form the perpective : have an idea : want board. fire up the program plonk down parts , some from lib , some i will need to make , route board, create gerber and send it out.
right now the libs are totally empty and the few parts that er there are wrong both as symbols and as footprints. you may as well not provide any library at all. That would have been cleaner.

[zapta]

Free electron, this review is very interesting. Would be interesting to get similar reviews on the other programs (eagle, diptrace and kicad and see how you rank them). 

[Stupid Beard]

Hey,

I've been lurking for some time, but just wanted to say ...

I'm a programmer. The kind of feedback that free_electron is giving is THE BEST POSSIBLE KIND OF FEEDBACK YOU CAN EVER HOPE TO GET. When I make something, it's the kind of feedback I expect to get and am extremely thankful for getting. Wanky "oh it's so great, thank you very much" feedback is completely useless. You need to know what pisses people off the most, because that's your priority #1 to fix. The same is true for any product, not just software.

Frankly, as an electronics hobbiest I am your target market for this kind of thing. I currently use Eagle because of all the affordable ones it pissed me off the least, but I would switch if something better came along that met my requirements. However, your attitude towards good feedback has kind of put me off even wanting to download autotrax. It certainly hasn't endeared me to wanting to give you money for it.

Anyway, I just wanted to thank free_electron for this thread. Actual bona fide good feedback can be a rare thing and should be welcomed. It makes me mad to see it dismissed because it doesn't fit with the developer's orgasmic view of their creation.

Hopefully Iliya comes to his senses.

[cjo20]

Hey,

I've been lurking for some time, but just wanted to say ...
<snip>

Pretty much what Stupid Beard said. It isn't encouraging when a developers response to "I have a problem with these features", even going as far as to include screenshots highlighting exactly where the problems were, is to ask what makes that person (in the target market for the product) qualified to review the software. It certainly doesn't make me want to spend money on some software if I have to submit a CV along with any bug reports.

Thanks for the review so far free_electron

[free_electron]

i managed to place some parts on the schematic. i downloaded that library installer. well that is a big pile of ... whatever. there are thousands of directories. most of them with 1 part in em .. 

running the search takes forever.

it SHOULD be :
if i start typing 0 all parts not beginning with zero are thrown out of the list.
08 all parts not beginning with 08 ar thrown out
08?5 all parts not beginning with 08 , then a wildcard and then a 5 are thrown out ( a trailing * should be implicit, no need to type that . a preceding * should NEVER be implict !)

so i can type for example 74??00 and get 74LS00 74HC00 74AC00 and so on ...
that list should be on the fly. symbols and footprints should also appear on the fly. so i can immediately see if this is linked against a dil or an SO or other package

here is how DEX works:

wildcards don't work
typing 74??00 gives a list beginning with MAX2700JD ... there isn't even a 4 in sight in that part number. search is flawed.
same for 74*00 ( according to the pop up balloon help wildcards are allowed , except they don't work.... . that search also gives a MAX2700JD as first part. my search query has the number 4 in it. a MAX2700JD does not have a number 4 in it so why do i get to see this MAX2700JD

see attached screenshots.

also the note clearly says that   *diode* is the same as diode.

type a single 0  : 56521 parts found.too many to list
now type *0   : nothing found
now type 0* : 110327 parts found. too many to list
now type *0* : nothing found

so that search wildcard thing not only doesn't work , it doesn't do what it says in the balloon tip ! (0 and 0* should be the same as *0* and it isn;t 3 different results : 5xxxx part, 11xxxx parts and no parts ... )

i can't figure it out.

is there a way to see symbol and footprint at the same time as opposed to have to click on those stupid tabs all the time ? can those tabs detach ? i'd like to see a parts browser where symbol footprint and 3d model are shown simultaneously. having to click back and forth all the time is very annoying.
i want to have to click one in the list and then simply use the arrow up and down key on the the keyboard to walk the list and pick what i finally need.

the library window can detach make it so that we can rearrange the tabs into individual panes inside that window as opposed to the static tabs.

some of the parts are ...  (picture 1) and no fingerpointing to an imported eagle library ! do your quality control please. you delivered this tripe. if i have a problem with my car body i do not want to hear that the supplier of the metal plate to build the chassis delivered rusty sheets.

And the list isn't even sorted properly... RESISTOR RESISTOR RESISTOR -RESIST RESISTOR Variable Resistor Resistor Resistor VariableResistor -Solid resistor ..

Can i at least see an alphabetically sorted list ? listview boxes typically allow you to sort up and down. This requires zero code from a programmer. The controls can do this by themselves. Can you make this list view have multiple columns so i can see not onl y the part name but also the filename and the footprint name associated with it in the same panel ?

here is why :
i may pick a 74LS00 and there will be 32 different ones listed. some will be in dil ,some in SO some in TSSOp ,some in DFN , some in QFN, some in CSP some in even other packages. i would like to be able to see in 1 shot what i have there so i can pick a part correctly. now it takes simply too much work.

3 columns : library name , associated footprint name, comment field
you can drop the footprint field if you can show me schematic symbol and footprint simultaneously without me having to click tabs.

oh and another annoyance :when starting dex ( after having to manually fix the shortcuts as those all try to launch the non-existing autotrax.exe ) :the program does not remember what monitor it was last on and what window state it was. it just appears random.
Also, your splashscreen pops 'under' i had chrome open. i am sitting there waiting and waiting for dex to load.. turns out the licence screen box was underneath chrome ...
please pop that up as FRONTMOST ( that is a form setting )

[Lightages]

Iliya:

You already know that I support you and your generosity in supplying your work for free. I also think that free_electron is supporting you but I know you don't see it that way.

What free_electron is doing is spending a considerable amount of time playing around with your software and giving you feedback, bad or good, from the viewpoint of a very experienced user of software like this. I know you find it insulting to have someone pick apart your work so brutally, but this is the best thing you could get. If a true professional user of this kind of software sees this problems, so will others. The way most people deal with something they see problems with is to just walk away the first sign they see of something that doesn't meet their expectations.

free_electron seems to taking a fair bit of time to give his opinion. Don't get insulted and take it personally. Take the information you are given and make use of it. It will benefit you in the long run. In business, hurt feelings are quickly compensated by more profit.

[free_electron]

Here is another thing i 'd like to see

i have placed 5 resistors on the schematic. i select 3 of them (shift-click) if i go to the parameter editor and change value to 1K only one of em changes. it should change for ALL selected parts. it is illogical that this changes only for one of em. there are 3 selected !

another thing that would be nice is the ability to quickly clone a part. let's say i have aresistor already on the schematic and the footprint and value are already set right. i need another one just like it. doing for example shift -drag  ( hold shift key , point mouse to existing part, press and hold left mouse key while maintaining shift held ) that 'clones the part being pointed at so i can immediately drop that where i need it.
now every time i need to go to the library panel and drag one from there. one that doesn't have the settings already in it ... so i need to redo that...

that shift-drag should work for any object. components, power objects , ports .. even a selected group should be cloned like that.

that speeds up drawing tremendously.