Creating a PCB layout

[adumas77]

Ok... I've now got a schematic that is working... Is there a way to export this layout into another package and have it auto layout a PCB? Is this the NetList to Ares option?
If so, what version will work and how much will it cost?

I don't need anything too fancy - I'm not building any rocket ships... I just need something that will save me time laying out the pcb.. I've been working with ExpressPCB and that's fine... But it seems that I should be taking the VSM schematic and having it do the work for me...

 

[Technical]

Please see the PCB tutorial available from the PICAXE VSM Software page.

You can use a netlist in lots of different PCB applications. We are not familiar with ExpressPCB but it may be able to import one of the netlist formats supported.

Alternately our recommendations for an alternate PCB application would be either ARES or realPCB.

 

[Mycroft2152]

As Technical said, the easiest method is to use ARES or Realpcb. VSM has a one click import to these programs. Importing to other pcb programs using a netlist can be done but is somewhat difficult.

If the pcb priogram cannot identify and match the component footprint with one it its library, it will ask you to select an equivalent. This has to be done each time you import a schematic.

Each component/footprint must have the identical name and pin numbers as in VSM.

I am finishing up a project that will allow exporting a VSM schematic to the free DIPTRACE pcb program. Here are the steps that it took:

1. Create list of unique VSM pcb componenet footprints (approximarely 75).
2. Redraw or rename DIPTRACE footprint to VSM names.
3. Convert pin numbers to match VSM component footprints.
4. Save all footprints into library.

At this point, I now have a one click method to import any VSM schematic into DIPTRACE pcb.

I have little experience with Expresspcb, I and more of a DIPTRACE and formerly EAGLE fan; but I took a quick look at importing netlists with Expresspcb. Using the Multiwire netlist format, you will have to recreate the components also.

Good Luck

Myc

 

[adumas77]

Thanks for answering... I would love to try out diptrace - something that doesn't cost me more money... I downloaded the latest version V1.4 - freeware.

I used the isis netlist command - I couldn't find diptrace so I exported using tango. Then within diptrace I picked import netlist tango file.

It came back saying something like "some components do not have attached patterns".

I'm clueless how to proceed. Can you help out?

 

[Mycroft2152]

As i mentioned in my previous post, the TANGO netlist has the ARES names and pinouts for the footprints. These do not match the "pattern" names in DIPTRACE. You can select "patterns' that may match in the drop down menu in the import page. (the VSN dsn file is ok too,)

Save your TANGO netist as a txt file and post it here and I will run it through my beta version of the DIPTRACE footprint library. I am not ready to release the VSM/DIPTRACE library yet.

I am waiting for for the final version of VSM to be released to make sure the VSM/DIPTRACE library is complete.

Myc

 

[adumas77]

Again thanks - and I apologize if I don't understand something - it's all brand new to me... But I like to think I a quick learner.

Here is the Tango.txt file.

 

[Mycroft2152]

Hi Adumas77,

Attached is the is your NETLIST imported into DIPTRACE pcb.

A couple of notes, The relay footprint was not availible, so I used the footprint of the standard P&B spst relay.

There also seems to be some pins are not connected. I checked the netlist and they are not listed. Post the dsn file for reference.

The forum will not allow the ".dip" pcb file to be uploaded so I changed the extension to "txt", you will need to change the "txt" to "dip" to open the file in DIPTRACE.

Myc

Yahoo IM Mycroft2152

 

[adumas77]

Hi Mycroft2152... It's great you are helping... I think we both want VSM to be successful - getting this to work with Diptrace would be great - if only to reduce the overall cost to hobbyists like myself. Spending $100 on VSM was quite a lot - I really don't want to spend another $100 - hard to reconcile with the wife...

Thanks for answering... Here is the dsn file... I physically moved every component and they seemed to be tied to the traces - so I'm not sure what is the problem vis-a-vis the pins...

 

[adumas77]

Just a follow-up... I saved the netlist file you uploaded and changed the extension to .dip... I then launched PCB and did a file open. It came back saying the format was incorrect.

 

[Mycroft2152]

The incorrect file format was my error. I have both Diptrace 1.40 and the 1.50 beta. I created the library in DIPTRACE 1.50beta, rather than the 1.40 version :0

I'm revising the library to 1.40 format.

Myc

 

[Mycroft2152]

The VSM simulator is a rather forgiving when running a design in the simulator. VSm will make certain "assumptions' to work.

Unfortunately, when exporting a netlist, all the "t's" have to be crossed and all the "i's" dotted.

All components must have designators (R1, C! etc) and associated fooprints.

The "ground" symbol does not connect automatically to the battery minus.

Batteries need a place to connect to on the pcb.

VSM has a component properties check box that "omits this component in the pcb", make sure the is correct for all components. the components that yopu want on your pcb should NOT have this box checked.

I suggest that you open the TANGO netlist in notepad and look at it.

-----------

HINTS:

Check to make sure all the components and packages are listed in the beginning.

Check that all the connections are listed.

----------

There may be some interference with the meters used to measure current and voltage on the pcb during netlist export. It seems they need to be removed before netlist creation. Finding this out was the result of just trial and error on my part. There were missing connections at those points. TECHNICAL, could you confirm this?

Overall, a good start, and just part of the learning curve.

Myc

 

[Labcenter]

I suggest that you open the TANGO netlist in notepad and look at it.

An alternative and perhaps more UI friendly way to check your design is to use the design explorer in netlist mode.

You can launch this via ALT+X or from the Design Menu. By default you get partslist view (physical components) which shows all the components together with their packagings but in this case you are likely more interested in netlist view.

At the top left of the design explorer are a set of icons - the second from the left switches into netlist (or connections) view with the right hand pane then showing a list of nets on the current sheet. Right clicking on any of the nets allows you to select which highlights all the wires on that net in the given sheet.

More info in the ISIS help file.

 

[Mycroft2152]

The Design Exploerer is very handy. but since we were discussing importing into pcb programs, looking at the netlist would be more appropriate for trouble shooting import errors.

In any event, while using the beta version of VSM for creating pcbs, it would be wise to check the Netlist and Bill of Materials when using a component for the first time. The libraries may not be fully fleshed out.

Hopefully, when the final version of VSN comes out, all components in the libraries will have an associated footprint. (OK, there will be some, like the meters and the IRLINK, that do not have a physical shape).

Myc

 

[adumas77]

Thanks for answering.. Sorry but I wasn't able to get back to this sooner...

I went through and checked the properties for each object. I deleted the simulators... And I ran a netlist for Tango... I looked at the output and it appears that everything was listed... But of course, I'm new at it so I might not be savy enough to know what is missing...

Here is the latest DSN that has been cleaned up...

Mycroft, will this work for diptrace?

 

[Mycroft2152]

Aduams77,

That looks a lot better. I'm on my way out the door, but I gave it a quick look. I'll spend some time on it when I get back this afternoon (it's 10AM now)

I think there are stiil a couple of problems to export the NETLIST to Diptrace or any pcb program.

It looks like the Vcc symbol puts both +5 and +12 volts on the same net. I don't think it's needed as you have the batteries on the schematic. Same goes for the gnd symbol.

How are you getting power to the buzzer? It looks like the Picaxe turns on the transistor and the transistor then grounds one side of the buzzer. The diode that is in the connection from the +12v to the other end of the buzzer, is reversed biased an will block the 12volts from the buzzer.

Myc

It is a good learning experience for both of us, we have to start somewhere.

 

[Mycroft2152]

Adumas77,

Well here it is -- finally. like many other things described as do-able in the literature, there were a few gotcha's.

Attached is a revised VSn simulator file, that exports a complete TANGO netlist that can be imported into a pcb program.

Also attached is the DIPTRACE (version 1.40) pcb file renamed as a txt file. Note; this is an unrouted pcb, I'm leaving the rest of the fun to you.

 

[Mycroft2152]

For those of you who do not have DIPTRACE pcb, here is a jpeg of the unrouted board

 

[Mycroft2152]

Now for the "gotch'sa", these are requirements for successful export / imports to ANY pcb program; ARES, Realpcb, DIPTRACE, and EAGLE.

To be fair, you'll find these requirements mentioned in a careful reading of the HELP files.

In VSM:
All components must have footprints (NULL isn't a footprint)
All component must have the checkbox "do not include in pcb" NOT checked.
All components shouoldhave pins identified with numbers or letters ( plus and minus signs do not work for exporting netlists)
Add battery connectors. the VSM simulator has some great shortcuts and is very forgiving and will work without batteries in the circuit.
Make sure your simulated circuit makes sense in the real world.

For the PCB [program:
All footprints must have identical names as in VSM.
All pin identifications must match exactly those in VSM.

Notes:

In PICAXE VSM beta, there are missing footprints for some components.

In PICAXE VSM beta, some pins are identified with a "+" or "-" sign, these will ot export/import coprrectly.

The PICVAXE VSM export to Realpcb has a fix file for some of the footprint / pin id problems, it is not complete.

Myc

 

[lbenson]

Myc,

I'm sure many have been following this thread with great interest. Thanks for being a real trailblazer here.

 

[Mycroft2152]

Thanks for the comment! It was a real challenge, and a lot of fun. Being able to create and simulate a PICAXE circuit and then transfer it to a pcb is fantastic.

The library is still in the beta stage, as there are a few more components that (I think) should be added.

I also want to recreate the library for use in making pcb's by the toner transfer method. For TT the pads should be a little oversized. The current footprints are matches to the ones in ARES.

Also any changes will also need to be made when the final version of PICAXE VSM comes out. Based on my license date, I'm guesing April 2008.

If anyone wants to try out the library, they can contact me through the private message part of the forum. I would appreciate the feedback.

Myc

 

[ArnieW]

Hi Myc,

I am at the steep end of the learning curve here - bought VSM a week ago and having great fun with it.

I'm now just beginning to think about making PCB layouts from VSM schematics and looking at options. It would be great if DIPTRACE and VSM can work together. I am a user of ExpressPCB but I'd rather not redraw circuits now that I have VSM.

How are you progressing on the DipTrace-VSM front?

and thanks for making this approach possible.

cheers, Arnie

 

[Mycroft2152]

Hi Arnie,

The guys at DIPTRACE recently updated the software to version 1.50, I've been using the 4.50beta, but want to check out the final version to make sure there are no problems. I'll be posting something shortly.

It would be worth you time to familiarize yourself with netlsts. Take a VSM design and export it anf look at the netlist in a text editor.

Make sure the properties of the individual components has the "use in pcb" box checked. Also each component must have an assoicatoed footprint.

The important part is that your pcb program has components with exactly the same footprint name and pin identifications.

Myc

 

[adumas77]

PCB Layout Update

Hi Mycroft... I'm just coming back to this thread... Last I time we talked you were figuring out the diptrace link...

Has this been all worked out? Is there a good link between the VSM and diptrace now?

I appreciate all the hard work you have been doing and have been holding off until you worked things out.

Right now I'm just using ExpressPCB and hand tracing everything. Kind of makes the VSM product only somewhat helpful. It is already a lot of money and without the PCB side of things, it is only somewhat useful. If this was exclusively for a business I might understand - but not all of us are doing it only for business... I hate to shell out another $100 - that's a lot of money.

Just let me/us know...

Appreciate it...

 

[Mycroft2152]

I'm pretty comfortable with the VSM/ DIPTRACE link exporting netlists from VSM into DT) now. I find it's a good combination.

There are a number of components in VSM that just do not have patterns (footprints), but those can be added in VSM pretty easily. Thats because the VSM libraries are not complete. There are a few others where the names of the pins cause some confusion.

But once you undertand these problems and how to get around them its pretty easy.

There is a bit of learnng curve, but I've got most of the sign posts worked out.

Myc

 

[Mycroft2152]

Adumas77,

Let me add to my coments about the library components.

The VSM simulator is a special limited version (subset) of ISIS for the PICAXE and was created by Proteus. Proteus also sells a professional pcb package called ARES (~$300US) that integrates directly with ISIS. When you purchased ARES pcb, you get all (?) the footprints for the components.

For Rev_Ed's educational customers, a less expensive pcb program was needed, REALpcb (~$100US).

Rev-Ed encountered the similar problems when trying to import netlists from VSM to REALpcb as I did with importing VSM netlists to DIPTRACE. Components footprints with diiferent names. Rev_Ed's solution was to create a translation file (in the .adi file in the VSM library folder).

Now this .adi translation file has a very limited number of components and uses the same footprint for different sized componets. It's was a compromise in the business sense and reasonible for the educational market. After all, why spend the money creating the conversions of 40,000 componets when under 100 will do.

There is a good explanation of exporting netlists in section 4 of the VSM tutorial. also, you can open the.adi file with any text editor to see the inner workings.

My approach for VSM/Diptrace was to create a Pattern (footprint) library of the components in the VSM PICAXE librarythat matched exactly the name used in VSM. That woould allow a direct import of the netlist without conversions.

There are some componets in VSM that need to have a footprint assigned to them, and some components need to have their name changed because a few components in VSM that do not use use the standard naming conventions for netlists.

It is not as difficult as it seems.

I hope this helps.

Myc

Myc

 

[rbright]

VSM/DIPTRACE Library

As i mentioned in my previous post, the TANGO netlist has the ARES names and pinouts for the footprints. These do not match the "pattern" names in DIPTRACE. You can select "patterns' that may match in the drop down menu in the import page. (the VSN dsn file is ok too,)

Save your TANGO netist as a txt file and post it here and I will run it through my beta version of the DIPTRACE footprint library. I am not ready to release the VSM/DIPTRACE library yet.

I am waiting for for the final version of VSM to be released to make sure the VSM/DIPTRACE library is complete.

Myc

Hello Mycroft2152 are you close to releasing the VSM/DIPTRACE Library?