DEX eval by free_electron

[aroby]

Nope.  Nothing happens.  I thought maybe it was the project I was using.  I created a new project, added a resistor to the schematic, then double clicked the symbol, the red bounding box, inside the bounding box.  The only double clicks that work are on the symbol name and value.  I'll submit a bug report.

Did you use resistors from "parts meny", if not, the "resistor edit" box wont appear.

Yes - I added a resistor from the parts menu, it displayed the Add a Resistor box.  I would now like to modify the footprint of that resistor, so I double click and would expect to get the edit a resistor dialog. 

[free_electron]

The danger of the 1 million+ part library

It’s a disaster waiting to happen on your project. Imagine how many mistakes there are in those parts.

If the library is correct (and not a clone from some other cad that is also flawed) : none
That is why you mark parts as 'released' or 'preliminary'. Once a part footprint is proven in production it gets toggled to 'Release'. That is part of the design cycle.

1) Create new part , mark as preliminary
2) make board
3) feedback : edit and go back to (2) or release part.

Basic design cycle management.

Even if there is just one part with the mistake and is the one you use then bang, there goes your first PCB.

- if the wizard is wrong then every board you make with it is wrong until the wizard gets fixed...

Now you can say, Ah! But I check all the parts I use by going and finding the datasheet and checking the part against is a datasheet.

No we don't . Once a part has been used once and verified to work it is marked as 'released'. Meaning known-good. Only newly created parts are marked 'preliminary'. Once we get the actual board made and all is well will we toggle this to 'Release'.

But I say wait a minute, why did you not go to the datasheet and use DEX’s superb part builder

- with a bug in it that creates wrong pinnames for BGA's. ... messing up every board over and over until the wizard is fixed...
- missing partbuilder for SON , PSON , WLPGA , VQFN , COB and a bazillion other parts. Should we put the pcb design on hold until we get the wizard ?
- Are you willing to write part builders for everything that exists out there ? This is not feasible. There simply are too many parts out there. Look at all the connectors ...  Grab the catalogs from digikey and mouser and see how many different parts are in there ... then go to websites for Molex, Tyco, Harting, Samtec and a thousand others ... it is undo-able.

give you an infinite combination of land patterns when you use it in your design.

We don't need infinite combinations.  We need 1 that is correct so we don't need to worry about it when doing a design. i vaguely remember an earlier version of dex that had an SMD part with a thru-hole footprint attached to it. Luckily i didn't make that board ...

Oh, I forgot to mention the time you waste looking for the part in the library, realising it is not suitable or even worse finding the part is not in the library.

-realizing there is no wizard.


So, in short : the other side of the medal :

- what if the part builder is wrong ?
- what if there is no builder for that particular footprint ?
- what if there is a known-good part : why do i need to go through the effort of recreating it over and over ?
- what if , late in the design we decide to change all 0805 by 0603 parts ? because they are cheaper, because we run out of room on the board, whatever reason

- What about the bill of material ? if you create all these parts dynamically : where is the bill of material information stored ?

We need a storage space for often used parts  , including all relevant data for that part ( order code, vendor, manufacturer, footprint , alternate footprint, symbol , alternate symbol. ) so we don't do work over and over. Having a working search filter makes searching very speedy. Of course if the search engine cannot handle a query like 74??00 and returns 555 in the results ...

At the end of the board design i need to generate:

- gerber data
- drill data
- paste data
- pick and place data
- a bill of material

This bill of material tells me exactly what part this is
- value , tolerance , voltage, manufacturer , part number, vendor, order code

So that there is no possible mistake when the board gets assembled. it will be the part we specified in the design.

Dynamically generating parts means we have to enter all that information by hand.
having a part in a library where the information is attached solves that problem.

If engineering decides we can no longer use yageo for resistor such and such (because it went obsolete, or its temperature range is not suitable, or it is not RoHs compliant or not whatever) they switch it the stackpole or roederstein.

During the output process the integrity checker will flag there is a discrepancy between design and library , in the bom area. The discrepancy gets resolved by pulling the new data into the design and the bom is now correct.

If we re-run an old design this flag pops up as well.

That is why libraries are one of the most important things in pcb design. Over the years almost every CAD package out there has evolved their library mechanism to a relational database so they can store all this info. It's all about design re-use, shortening the design cycle and incorporating feedback.

I believe you use an XML based system. let me try to give you an idea of how you could implement such a mechanism very easily. XML is extensible by nature.

Imagine an XML file named 'DEX_Library'

Code: [Select]

<XML>
<FOOTPRINT  R0805>
    ... xml code that allows to generate the graphics for this footprint
</FOOTPRINT>
<FOOTPRINT R0603>
    ... xml code that allows to generate the graphics for this footprint
</FOOTPRINT>

... more footprints here

<SYMBOL Resistor>
    ... xml code that allows to generate the graphics for this symbol
</SYMBOL>
<SYMBOL Capacitor>
    ... xml code that allows to generate the graphics for this symbol
</SYMBOL >

... more symbols here

<PART 1K-1%-0805>
  <USEDSYMBOL> Resistor </USEDSYMBOL
  <USEDFOOTPRINT> R0805 <USEDFOOTPRINT>
  <DATASHEEt> Roederstein.pdf </DATASHEET>
  <VENDOR> <NAME>Digikey</NAME><PARTNO>472-155-1-ND</PARTNO> </VENDOR>
  <VENDOR> <NAME>MOUSER </NAME><PARTNO> 722-485222<PARTNO> </VENDOR>
</PART>

... more parts here

This would allow for storing multiple footprints and symbols in 1 file and have all other relevant data in there as well.
The crosslink data is in the <PART> definition.

If i alter the R0805 then all parts that relate to that are automatically updated as well. Fix once, fix forever.

This would be the library file.

In a design you would have:

Code: [Select]

<DESIGN foobar>
<footprint>
   ... xml code to create repsentation of the footprint
   <ROOTOBJECT> machine_id+path+libraryname</rootobject>
</footprint

<symbol>
    ...
   <ROOTOBJECT> machine_id+path+libraryname</rootobject>
</symbol

<part>
    ....
   <ROOTOBJECT> machine_id+path+libraryname</rootobject>
<part>

<wire>
</wire>
</design>

As the design file holds a copy (the local cache so to speak)  you can open this file anywhere. All required data is in the design file.

If an integrity check is run you can use the <rootbject> to see if you can find the original library and run a compare between the data stored in the design file and the data in that library. If there is a mismatch you can present a report and the designer can accept/reject changes.

This is how the big cad software does it (Mentor, Cadence , Altium you name it)

The physical implementation can be a file system , a Database system ( Access, Excel ) or something proprietary. Some of these systems even have version control so they not only store the footprint but also all revisions of that footprint and you can roll backward and forward and see what modifications were done over the lifespan of that footprint or symbol.

Some symbols have alternates ( for example IEEE versus ISO representation of an AND gate )
 

[Iliya]

Iliya, from the feedback of seasoned PCB CAD users, it seems that there is a genuine need for an option, at least, for a split database for symbols and footprints. Is your reluctance to implement it due to difficulties with software modifications or a conviction that a change is unnecessary?

The problem is not software modification it is I just don’t see the point.

What I’ve been considering is a relational database containing tables of parametric part parameters. DEX is capable of automatically creating schematic symbols, footprints and 3-D models from a small number parameters. So the database will be extremely small in size but it would be very easy to add parts by simply adding parameters such as pin names and the associated symbol terminal name together with package type. The pin names and symbol names can be captured from PDF using DEX’s capture. I’m considering using MySQL or SQL Server.

An easy way of constructing the tables will be to use a spreadsheet. DEX already has a spreadsheet so it will be a simple matter of using this to edit the tables. The spreadsheet will allow you to enter formulas to create a series of parametric parts.
So the DEX librarian would consist of a spreadsheet coupled with 2-D schematic and footprint views and a 3-D view. This could be coupled with a Web server and allowed distributed part management.

Additional data could be associated with a parametric’s such as manufacturer details, suppliers, costs.

The relational database will also allow version control.

[Monkeh]

Iliya, from the feedback of seasoned PCB CAD users, it seems that there is a genuine need for an option, at least, for a split database for symbols and footprints. Is your reluctance to implement it due to difficulties with software modifications or a conviction that a change is unnecessary?

The problem is not software modification it is I just don’t see the point.

Spend a few years doing production designs.

[Iliya]

Apart from the basic parts, I always seem to spend most of my time creating new parts.  It would be handy if there was a small library of common symbols to choose from, to reduce the time spent drawing symbols more complex than a box or a triangle.

There is a library of common symbols. See below. Just drag the art symbol into your schematic.

You can add your own symbols by simply selecting them and then selecting the graphics and right clicking in the librarian and select add graphics. You can also modify any graphics that you have then save it.

[aroby]

There is a library of common symbols. See below. Just drag the art symbol into your schematic.

You can add your own symbols by simply selecting them and then selecting the graphics and right clicking in the librarian and select add graphics. You can also modify any graphics that you have then save it.

Got it, thanks!

[free_electron]

The problem is not software modification it is I just don’t see the point.

And that is the root of why you get so many comments , and why people are bitching and moaning.
You implement things the way you see them. And that is fine, it is your software after all, you control it.
The problem is you don't have a solid grasp on the entire problem or the entire design cycle. The implementation you make is based on your perception.

change is good and welcome , but only if it fixes a problem, not if it creates 20 new problems.

What I’ve been considering is a relational database containing tables of parametric part parameters.

in itself not a new idea. That is how component libraries have been made for decades now. Your new idea is the parametric portion. That could be a good idea , provided there is a mechanism to override the parametric portion and apply customisation. There are simply too many footprints out there. You can parametrize something like an SO package : 2 rows two colums, specify pad size and pitch and done. But, even with such a simple item : i want pin 1 to have a different shape than the rest so my pick and place vision system can detect it and use it as local origin. ( removing the need for a local corner fiducial ). So now we have another parameter in the 'pool'. I may want to shrink paste, or remove soldermask because i am using thick copper on my board and the fab cannot print the soldermask. So now we have another parameter.

The problem in board design is that there are more exceptions than 'norm'. and that makes parametrized parts very difficult. You can use them as the base ( that is what the wizards do) but you can not take away the ability to fully customize them. You , as the software designer, have no idea what the user may need to tweak in the part. you do not know his assembly or production process. there are simply too many variables.  So you can automate only to a certain point. They may have a super secret manufacturing technique that they are absolutely not sharing with the rest of the world. you can not know, and you can not make assumptions. The software can not limit because of what the software designers thinks is not necessary. It can of course limit because the software designers may not know how to do something or have not implemented it yet. But there can not be an 'apple' stance where they go : you don't need that. That is not up to them to decide.

All PCB cad software these days has a large set of common functionality. That is the starting point.
Differentiation between tools lies elswhere

DEX is capable of automatically creating schematic symbols,

I doubt that heavily. If i feed a part number to DEX : how does it know if this is an opamp or a timer ?
Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

In your perception symbols are generated 'automatically' because all you need is a rectangle.
That is not what the rest of the world works. If all we needed were rectangles we would have stopped drawing capacitor symbols and diode symbols long ago. Why go through all the trouble  ? simply draw everything as a rectangle. it's less work. But there are reasons why we have all kinds of symbols, even if that means a bit extra work.

Let's take a large step back and look at something else first.

Historically drawing CAD software began by allowing you to draw some lines and dots and send those to a plotter. the computer software was a replacement for decon-dalo rub-on pads and masking tape. it saved work.

Then we started building libraries with often used symbols and footprints to save time.
Over time other data was introduced : the link between symbol and footprint. procurement data, variants, alternates , stuffing options, spice models, 3d models, s parameters, IBIS models, thermal models.

Today we live in a data-driven design world.
We are now at the point where all information relating to a design , down to procurement data, is stored in a database. the symbols and footprints themselves are just one more property.

we have evolved from the concept of having a symbol and a footprint and "we'll fill in the blanks later" to a model of

here is a part
- this is the footprint
- this is the symbol
-thsi is the spice model
- this is 3d model
- this is who  makes it and the part number
- this is where we buy it.

We have gone beyond that to the point where some of this information meshes with other databases , for example live data from our vendors. our database holds the order code, so our database should be able to launch a query to our vendors database for the current price, in different quantities. Ideally our database or the vendors database has crossreferencing so it may suggest a cheaper alternative.

so now we deal with meshing databases with non-static data. everything is 'live'.

if a root element gets updated ( could be the price, could be the silkscreen on a footprint )  this propagates realtime to new designs and can be backported to existing, on-going or old designs.

There should be no duplication of data in the 'master database'. That is why everything is relational in there.

In the design we are faced with the problem that we cannot deal with data that can alter at a whim. So we use a cached copy. a snapshot in time from the master database. This allows us to do the work. Before we send it out for production we do a compare against the master databases and fix or reject discrepancies. ( we may reject a vendor change for a part because we still have 20 reels of the old one and we will use those up first and then we will change). we may reject a footprint because our board has a special feature that requires a tweak on this instance.

That is why the data pertaining to the design is stored in the design.  It is pulled from a master database and can be verified and update if we desire so. It can also be locally overridden and left.

We are now at a point in time where there is a clash between design and manufacturing. The 'old skool' way of doing things by exchanging odb and gerber no longer are sufficient. There is not enough info in those formats. if the production house finds a problem they flag it we need to change it and send data back. we need a mechanism where they suggest the change and we can click 'accept' and our database gets fixed.  This de-duplicates work and maintains the integrity of the data .  It is all about collaboration.

That is why now IPC has made a new data exchange standard (2581) that holds the entire design in a vendor neutral format. I can save my entire project as IPC2581 from cad program x and cad program Y can read in this design and reproduce it completely and correctly.

So now if the fab house needs to do a tweak : they alter the data and send back the design. i can compare revisions and accept or reject changes.

Just like in a word document you can put tags and revision and edit information this can now be done in the electronics design world. I can read someones document, propose changes and the other guy can approve or reject. I have access to the root data.

Of course this brings in new problems. Having access to the every aspect of the design means it could 'walk off' to the competition very easily.  that is why 2581 has provisions to mask off data. i can block the schematic or where i buy my parts , or my price. At that point a subset is created which is task specific. But, i can re-import that subset, and changes, back into my master design file so it still saves me a lot of work.

Designing a lump of electronics is no longer divided into a schematic,  a pcb, a collection of parts, a procurement database, an alternate part , a collection of papers and post it notes and 'only Kathy knows where to find that piece of information'

The design itself is stored as an entry linking to live or cached data and there are multiple ways in and out of this database, each with their own checkpoints.

Some of that stuff can be automated ( like meshing between my database and a vendors database to get live price and stock info). some of it can't as it falls in the 'exceptions' category ( customized symbols, customized footprints )

We are evolving even beyond this point. Component manufacturers already give us accurate 3D models so we can make sure stuff will fit. In a lot of instances manufacturers also begin by giving us the actual footprints and symbols. This can be in a vendor specific format ( today) but is moving fast to a vendor neutral format that any cad program will be able to read (2581 is the ideal candidate there)

Pick part from a website and the symbol and footprint appear automatically. These are vendor verified. any error is immediately corrected so the trust in this data is very high.

This is not 'future music'. It is here today. The industry uses it, and not only the big boys. Lots of small companies cannot afford hiring someone to do procurement, another guy to do inventory, another to do x y or z. If there is a piece of software that can handle the 'annoying bits' , that is what we will go for.

stuff to think about.

(typed with two fat fingers on a keyboard)

[Iliya]

There is a library of common symbols. See below. Just drag the art symbol into your schematic.

You can add your own symbols by simply selecting them and then selecting the graphics and right clicking in the librarian and select add graphics. You can also modify any graphics that you have then save it.

Got it, thanks!

what I often do is use the part builder to create the part and use the part builder's symbol capture to capture the symbol names. Then I go into the symbol select the symbol border and press delete. Now add your graphics from the library and place the terminals where you want them. Then save and use.

[Iliya]

Checking your work

DEX has an extremely valuable tool call the checker. This is a dockable control panel that allows you to select electrical items in schematics and the PCB and mark them as checked. The checked items appear as if a marker pen has being drawn over them. Below you see an electrical node that has been checked off and has a marker drawn all over the wires. Similar marking can be applied to all symbol terminals.

The checker currently does not work in the part editor which is a shame so I will be adding that functionality very shortly.

[free_electron]

Checker : Great idea ! love it 

[Iliya]

Checker : Great idea ! love it 

The idea is to be similar to printing out a hardcopy and taking a marker pen to it. But with DEX you get to save the markings with the file. The marking can be made invisible and in fact is simply a Boolean flag on the electrical item to say they are checked. Optionally when you select an item in the checker you can get the checker to find the sheet item is on and auto zoom.

It works with tracks on your PCB.

[rsjsouza]

Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

Just a tip. Check the video below where a part is split and edited in three schematic sheets.


In the video you still have the three rectangles, but they could potentially be modified into circles, triangles, etc.

The trick is if the splitted part can be saved to the library. It probably can, but I did not explore this.

[free_electron]

checker : can you also check parts ? like if a part was approved and verified : mark it as checked.

[Iliya]

checker : can you also check parts ? like if a part was approved and verified : mark it as checked.

as I said earlier I have yet to do it for the part editor. But I intend to do it. What I will check for includes:

schematic symbol
for each symbol terminal check symbol name, pad name.
Reference designators
part value

Footprint
courtyard
silkscreen
placement point
for each pad check shape, size, position, hole size, pad type SMT/TPH

Any further ideas?

[Monkeh]

Does it automatically reset the checked status if you modify the net or part?

[free_electron]

checker : can you also check parts ? like if a part was approved and verified : mark it as checked.

as I said earlier I have yet to do it for the part editor. But I intend to do it. What I will check for includes:

schematic symbol
for each symbol terminal check symbol name, pad name.
Reference designators
part value

Footprint
courtyard
silkscreen
placement point
for each pad check shape, size, position, hole size, pad type SMT/TPH

Any further ideas?

my question was in the part editor but in the schematic.  Someone could double check the wattage and footprint is right (for example) and mark the part as 'ok'.

[Christopher]

A simple parameter for each part would be good, we use

"checked?" (y or n)
"checked_by" (initials)
"checked_date"

we also use approved as we all know what happens when we check our own work.

That way you know who to blame when it comes down to the PCB being wrong when it comes in 


A good feature would be when the part is modified and saved, to change the checked parameter to no. Or save a last edited date.

[Wytnucls]

Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

Just a tip. Check the video below where a part is split and edited in three schematic sheets.


In the video you still have the three rectangles, but they could potentially be modified into circles, triangles, etc.

The trick is if the splitted part can be saved to the library. It probably can, but I did not explore this.

Did you try it? Because it doesn't work for me. I can make a sibling, but when I try to move it to the bin or delete it, it just disappears and the parts bin stays blank. (Using an ATMEGA88-20PU from the library) (DEX 5.05)

[rsjsouza]

Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

Just a tip. Check the video below where a part is split and edited in three schematic sheets.


In the video you still have the three rectangles, but they could potentially be modified into circles, triangles, etc.

The trick is if the splitted part can be saved to the library. It probably can, but I did not explore this.

Did you try it? Because it doesn't work for me. I can make a sibling, but when I try to move it to the bin or delete it, it just disappears and the parts bin stays blank. (Using an ATMEGA88-20PU from the library) (DEX 5.05)

No, I didn't. I didn't have yet the need and assumed it worked given the video was showing the procedure.

[Iliya]

Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

Just a tip. Check the video below where a part is split and edited in three schematic sheets.


In the video you still have the three rectangles, but they could potentially be modified into circles, triangles, etc.

The trick is if the splitted part can be saved to the library. It probably can, but I did not explore this.

Did you try it? Because it doesn't work for me. I can make a sibling, but when I try to move it to the bin or delete it, it just disappears and the parts bin stays blank. (Using an ATMEGA88-20PU from the library) (DEX 5.05)

Oops! There was a bug when splitting the part and moving the split part to the parts bin. It is now fixed and I'm uploading the new software. Give it about 10 minutes after this posting.
I apologise for the problem.

[Iliya]

Does it automatically reset the checked status if you modify the net or part?

Sorry no it doesn't. I will add the check unset when modified to the to-do list.

[Monkeh]

Does it automatically reset the checked status if you modify the net or part?

Sorry no it doesn't. I will add the check unset when modified to the to-do list.

[Wytnucls]

Your idea of a IC symbol is a rectangle with pins. That is a very narrow view.  I may want to split the device in mulitple parts so i can put one section on page 1 and another section on page 7.
section one is drawn as a circle with a cross in it (could be an analog multiplier) while section two is a triangle (opamp).  so this 'auto generation does not work , unless all you create is 'blobs'.  That is not how schematics are drawn. A schematic needs to be readable. Drawing everything as simple rectangles
doesn't work.

Just a tip. Check the video below where a part is split and edited in three schematic sheets.


In the video you still have the three rectangles, but they could potentially be modified into circles, triangles, etc.

The trick is if the splitted part can be saved to the library. It probably can, but I did not explore this.

Did you try it? Because it doesn't work for me. I can make a sibling, but when I try to move it to the bin or delete it, it just disappears and the parts bin stays blank. (Using an ATMEGA88-20PU from the library) (DEX 5.05)

Seems to work now. There is a quicker way to split the symbol. Select required pins, right click and save to 'new sibling symbol'. Then move the new sibling symbol to the parts bin, followed by a move to the secondary schematic. Perhaps a bug still: all the symbol parts moved to the bin, but they can be repositioned on the right schematics afterwards.
Even quicker: If 'move to sibling symbol and add to parts bin' is used instead, then everything is fine, as the previous symbol parts stay in place on their respective schematics.

[CatalinaWOW]

There are at least three parts to the checking problem that I see.  One part can and should stay with the user in my opinion.

Part 1.  Checking the schematic.  DEX does this for traces now, and it appears that Ilya is heading for some marking on the symbols to verify that the part is checked.  This should be the check that the correct package, part grade etc. for the application is the one used.

Part 2.  Checking the part.  DEX seems to be heading for a variant of the schematic checking for the parts checking.  I don't think it will mechanize as easily, but assuming that it does, this will be the place to make sure that footprints, symbols, etc. are consistent with the part designation.

Part 3.  Verifying that only checked parts are used.    While you could use unchecked parts and then let force the program to do any back annotation etc that occurs due to corrections which occur in the check process, I see much evil that would come out of this approach.  The only process I have seen work is to get the parts right first (or at least very early in the process). 

DEX supports local and user librarys.  It is easy to create on for each project, and populate it only with checked parts - whether these have been checked using future tools from DEX, or the old fashioned way with brain cells, print outs and pencils.

[Mechatrommer]

Oops! There was a bug when splitting the part and moving the split part to the parts bin...
I apologise for the problem.

now my friend, accepting mistakes will not make you weak, but stronger instead. i wish dex one day become on top of the line with this kind of attitude. i still have major (but basic) feature request before it become usefull to me, but who am i i dont have a phd...

a little hint, automatic wiring as already mentioned, please let the user wire or route manually. routing new or moving existing tracks in pcb with 45degree angle with "move with parallel" thats the default behaviour of every single board i found in my store, make that as default please, there must be a reason for it, every single person on earth doing it they mustnt be fool, thinking otherwise is a delusion. please remove nasty feature like auto re-arrange component pins after we manually placed them as f_e already mentioned, thats unthinkable, i dont know how a programmer can come up with that idea in todays world (overriding user's setting), and then secondly, a workable simulator (please see and feel how tina-ti works) be able to set V,I source parameter etc. about 3d, no objection there its nice, but if you can add insertable additional 3d objects such as casing/enclosure, other misc stuffs usually mechanical stuffs be put together with pcb, with precise/numeric placement. capable of cut-out/split view for presentation or collision examination, that can be a big plus of the decade. 3d area seems too easy for you. thirdly, another area nonexistence... push and shove, diff/bus routing, impedance control, mixed signal simulation, signal integrity, rf/microwave area maybe, but forget that for a moment, concentrate on more important stuffs for beginners mentioned earlier. no use of putting advance stuffs if basic stuffs is broken. and lastly documentation, documentation, documentation! you already did some but not enough, making people trying it wonder about misbehaviours, is it a bug? missing features, users mistake, system incompatibility or what?

otoh if you learn to listen to what users need, you'll have their money 50,100,200 or even more depending on the usefullness. if you brag, live in your own reality, nobody give a sheet no matter how holy the dex is (only the weak minded be seduced by the dark side of the force). i know it will not be tomorrow or next months, but one day i hope dex can be a success, just keep the manners and sanity in checked. the one most greatest thing about dex is.... you are here! fwiw.,