Author Topic: Can you use CS without a schematic ?  (Read 4421 times)

0 Members and 1 Guest are viewing this topic.

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Can you use CS without a schematic ?
« on: August 02, 2016, 04:14:53 pm »
Just started looking  at CS - been using PCAD for many years.
My normal design flow does not start with a schematic ( there are many reasons for this - will probably do a vid sometime!).
I put down parts & pads, create nets within the PCB layout by rubberbanding between , then place & route.
I've been playing around with CS and can't immediately see a way to work like this - I've not found any way to create nets within the PCB editor.
Is this workflow possible in CS?
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline trophosphere

  • Regular Contributor
  • *
  • Posts: 217
  • Country: us
Re: Can you use CS without a schematic ?
« Reply #1 on: August 02, 2016, 04:41:10 pm »
It is possible to create nets within the PCB editor.

With a blank pcb file opened, go to the ribbon menu and navigate to Tools>Netlist>Edit Nets... This will open up a dialog box that will contain all nets in your pcb. Hit the 'Add" button and then fill out the needed information - e.g. net name, trace width, and via sizing. Click the "Okay" button and the newly created net should then appear in the first list box.

Assigning nets to pads can be done by double-clicking on the pad of interest to get into the properties dialog box and then selecting the net under the properties section.
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #2 on: August 02, 2016, 06:22:50 pm »
It is possible to create nets within the PCB editor.

With a blank pcb file opened, go to the ribbon menu and navigate to Tools>Netlist>Edit Nets... This will open up a dialog box that will contain all nets in your pcb. Hit the 'Add" button and then fill out the needed information - e.g. net name, trace width, and via sizing. Click the "Okay" button and the newly created net should then appear in the first list box.

Assigning nets to pads can be done by double-clicking on the pad of interest to get into the properties dialog box and then selecting the net under the properties section.
I'd figured out the latter after importing a PCAD design, but that whole process is tedious enough to be a complete dealbreaker.
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline Someone

  • Super Contributor
  • ***
  • Posts: 2169
  • Country: au
Re: Can you use CS without a schematic ?
« Reply #3 on: August 03, 2016, 12:35:38 am »
Its possible to turn off the short circuit checking and draw PCBs freehand without a netlist, I've done this in Protel for some simple designs that are more constrained in shape/position than in PCB design rules. Just to check for you I fired up AD and put some parts down, you can freely draw in connections between parts but the "Create Netlist From Connected Copper" command doesn't seem to function but "Configure Physical Nets" did assign nets to all the connected copper and then the design rules all run normally. You could very well run "Configure Physical Nets" periodically while routing and do a board entirely without a schematic and still end up with a good coverage of interactive and offline design rules.
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #4 on: August 03, 2016, 09:07:09 am »
I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing. ,

Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Online tautech

  • Super Contributor
  • ***
  • Posts: 16356
  • Country: nz
  • Taupaki Technologies Ltd. NZ Siglent Distributor
    • Taupaki Technologies Ltd.
Re: Can you use CS without a schematic ?
« Reply #5 on: August 03, 2016, 10:11:49 am »
I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing.
Altium isn't much different, a trace or pad double clicked will show Properties in which nets can be assigned.
A free pad or trace Properties will show as "No Net" within a netlist box and existing nets can be assigned to your new pad or trace.
I've used this on the odd occasion when library parts haven't linked correctly and also when you need a quick fix to a routing problem with multi gate logic packages and aren't worried about updating the schematic as you can do it later from the finished PCB.
Avid Rabid Hobbyist
 

Offline Someone

  • Super Contributor
  • ***
  • Posts: 2169
  • Country: au
Re: Can you use CS without a schematic ?
« Reply #6 on: August 03, 2016, 10:27:37 am »
I don't often want to draw without a netlist (although this can be useful for things like large arrays), I want to create the netlist quickly and easily within the PCB editor.
With PCAD, I go into  "place connection" mode, drag a connection line between pads - if it's a new net it pops up a dialog with a default net name (NETxxxx) , which I can either edit or just hit enter to use the default.
I can also right-click on a pad and do "add to net" from a list of the nets in the design.
As for DRC, it can manually route using the design rules so you generally end up with most rules met. Subsequent dragging of parts & tracks can break the rules but you can just run manual DRC which tags issues for manual fixing.
Altium isn't much different, a trace or pad double clicked will show Properties in which nets can be assigned.
A free pad or trace Properties will show as "No Net" within a netlist box and existing nets can be assigned to your new pad or trace.
I've used this on the odd occasion when library parts haven't linked correctly and also when you need a quick fix to a routing problem with multi gate logic packages and aren't worried about updating the schematic as you can do it later from the finished PCB.
Adding pins to nets manually is useful for exposed pads or odd connectors with many mounting pins that you want to use as conductors/vias. But back on the OP there isn't an easy way to create named nets (that I know of or could find), seems like Mike has a very specific workflow in mind which isn't possible as far as I can see.
 

Offline NANDBlog

  • Super Contributor
  • ***
  • Posts: 4485
  • Country: nl
Re: Can you use CS without a schematic ?
« Reply #7 on: August 03, 2016, 10:28:47 am »
Altium's normal design flow was always SCH->PCB. You will save yourself from a lot of headaches if you follow this. I believe the correct way is to set the pads to a net, and then just connect them together. I think you have to select the pads you want to connect, open the PCB inspector panel, and then enter a net name to the net. But be prepared that this will make your life very hard, with a lot of issues.
I'm not sure if CS has pin swapping support, but I assume that is one the reason you want to do it this way.
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #8 on: August 03, 2016, 10:30:43 am »
It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot. 

Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline NANDBlog

  • Super Contributor
  • ***
  • Posts: 4485
  • Country: nl
Re: Can you use CS without a schematic ?
« Reply #9 on: August 03, 2016, 11:04:50 am »
It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot.
Yes, in CS it will be a pain in the arse. In Altium you make a SCH with a single LED or some LEDs, place multiple SCHs as a sub sheet,a so called "room" is created, then you route it, and then just "copy room" so the routing on all the rooms are the same. CS... forget it, that would be productive.
Also, there is the SCH list, where you can just copy from excel (or whatever) the location info for a component or a net. That is gone in CS.
I'll try to think something, but I only had CS trial license. Did you buy it or just trying?
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #10 on: August 03, 2016, 11:35:09 am »
It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.

If you're doing a PCB with >1K LEDs (on 2 layers) , this stuff matters rather a lot.
Yes, in CS it will be a pain in the arse. In Altium you make a SCH with a single LED or some LEDs, place multiple SCHs as a sub sheet,a so called "room" is created, then you route it, and then just "copy room" so the routing on all the rooms are the same. CS... forget it, that would be productive.
Also, there is the SCH list, where you can just copy from excel (or whatever) the location info for a component or a net. That is gone in CS.
I'll try to think something, but I only had CS trial license. Did you buy it or just trying?
They gave me a freebie - Dave emailed me to let me know they were desperate for bloggers etc. to look at it.
With a few small additions it could be a good solution - I don't think there's anything fundamentally broken, just that they'd not considered a layout-centric design entry method.
I think a reason that PCAD originally made this easy is that you used to be able to buy PCB seperate from schematic.
 
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Offline NANDBlog

  • Super Contributor
  • ***
  • Posts: 4485
  • Country: nl
Re: Can you use CS without a schematic ?
« Reply #11 on: August 03, 2016, 02:36:06 pm »
Creating a component - from the PCB section you want to multiply - could work. Only your Pick & Place file and your BOM will need some work afterwards.
I also see "create netlist from connected copper" in the netlist menu. Basically turn off online DRC, connect what you want, create netlist, update SCH, enable DRC. Maybe you need to go to PCB rules and disable the short circuit rule for the time.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7242
  • Country: us
    • SiliconValleyGarage
Re: Can you use CS without a schematic ?
« Reply #12 on: August 03, 2016, 02:41:24 pm »
place LINE

wire up board

then pull a netlist from the board.
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #13 on: August 03, 2016, 02:52:37 pm »
place LINE

wire up board

then pull a netlist from the board.
Quote
I also see "create netlist from connected copper" in the netlist menu
That would be the equivalent of PCAD's "reconnect nets", which creates or merges nets based on previously placed tracks.
Just tried in CS, and it doesn't appear to work, at least not how I'd expect - after doing "create netlist" I'd expect to see teh new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

« Last Edit: August 03, 2016, 03:07:33 pm by mikeselectricstuff »
Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Online tautech

  • Super Contributor
  • ***
  • Posts: 16356
  • Country: nz
  • Taupaki Technologies Ltd. NZ Siglent Distributor
    • Taupaki Technologies Ltd.
Re: Can you use CS without a schematic ?
« Reply #14 on: August 03, 2016, 06:55:44 pm »
I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part
How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?
Avid Rabid Hobbyist
 

Online mikeselectricstuff

  • Super Contributor
  • ***
  • Posts: 12050
  • Country: gb
    • Mike's Electric Stuff
Re: Can you use CS without a schematic ?
« Reply #15 on: August 03, 2016, 08:17:46 pm »
I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part
How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?
Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.


Youtube channel:Taking wierd stuff apart. Very apart.
Mike's Electric Stuff: High voltage, vintage electronics etc.
Day Job: Mostly LEDs
 

Online tautech

  • Super Contributor
  • ***
  • Posts: 16356
  • Country: nz
  • Taupaki Technologies Ltd. NZ Siglent Distributor
    • Taupaki Technologies Ltd.
Re: Can you use CS without a schematic ?
« Reply #16 on: August 03, 2016, 08:22:39 pm »
I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part
How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?
Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.
Ah, now I see why you liked PCAD for your work flow.  :)
Avid Rabid Hobbyist
 

Offline Someone

  • Super Contributor
  • ***
  • Posts: 2169
  • Country: au
Re: Can you use CS without a schematic ?
« Reply #17 on: August 04, 2016, 03:48:54 am »
It appears to be possible, but way too cumbersome.

I also can't see any way to create regular arrays of parts, or copy/paste repeated sections of a circuit with net creation/merging.
I've not had many problems with the "smart" pasting merging/reassigning nets based on what you're dropping it onto.

I'd expect to see the new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part
How can that happen unless the same net class is assigned to both?
Without a net name for both, no way.

Does the package you used before auto assign a net to a new pad when connected by copper?
Yes - if any uncommitted pad intersects an uncommitted track or polygon, a new net is created with a name of the form "NETxxxx" where xxx is an incrementing number. If an uncommitted pad intersects a track that has a net, that pad is added to that net.
Class would be whatever is the default.
If you don't mind the nonsense net names of "NewNetxxx" then the above workflow using the "Configure Physical Nets" works, but you'll have to manually add pads if you want rats nests along the way, the rats nest will appear on routed nets after each "Configure Physical Nets". Renaming of nets automatically propagates so you can add some readable names as needed.

Once there is a named net on some copper you can't connect any of the "No Net" primitives to it with normal interactive routing turned on, turn off the push/avoid routing and you can flow copper anywhere you like and nets will merge automatically though the "Configure Physical Nets" along with allocating pads and copper.

This is all with AD, some or any of the options might be missing from CS.
 

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7242
  • Country: us
    • SiliconValleyGarage
Re: Can you use CS without a schematic ?
« Reply #18 on: August 06, 2016, 05:26:05 am »
place LINE

wire up board

then pull a netlist from the board.
Quote
I also see "create netlist from connected copper" in the netlist menu
That would be the equivalent of PCAD's "reconnect nets", which creates or merges nets based on previously placed tracks.
Just tried in CS, and it doesn't appear to work, at least not how I'd expect - after doing "create netlist" I'd expect to see teh new net on the part pads I'd drawn the line to, and to see a connection rubberband if I then moved the part

once youcreate such a netlist you need to push it. do a net-clean all. ( dont know if it exists in CS but it does in big altium.)
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf