Cadstar some Diverse Question

Hi

i have some question about cadstar that not find anser

1-) in Schematic for assing net route code
need to go net -> propriety -> net -> then change net code in pull down menu

did it have any other way to make that and permit edit many at once ? (like for attribue whit attibut editor)

2-) for Generate Gerber whit batch process

any way to got output file match desing file or other Feild
in other word each time i generate gerber for a new design it
overrite last one so that may dagerous to screw files ..
or keep one .ppf file for each design that also error prone
(i look for generate the .ppf by report genrator but must have better/simpler way ?)

3-) i read a ton of post about vanising via issue and idea to let it whit small section of trace
but did since recent year did have any other solution comming ?
that very annoying since i use lot of via on copper pour and themal pad of QFN
and even fixed it varnish , cannot belive someting so simple as put multi via on a same templace
was not handele right ? (and possibility add free via then add a net to it)

4-) any way to set placememt goup attribue in sheamtic (used for replicate placement)
on pcb it easy to select part -> attribut editor -> then back anotation in SCH

if try to do same on schematic (select part then attribut editor)
i not find any o the attribue that replicate placement handel ?

Best regard
Marc L.

T5400 said:

Hi
i have some question about cadstar that not find anser

1-) in Schematic for assing net route code
need to go net -> propriety -> net -> then change net code in pull down menu

did it have any other way to make that and permit edit many at once ? (like for attribue whit attibut editor)

Click to expand...

No, there is no other way.
ISTR that I have asked for this as an enhancement.

Generally the scm is created using the default route code and then only those that need changing are given another route code, you can group select nets using "select net" to do this.

T5400 said:

2-) for Generate Gerber whit batch process

any way to got output file match desing file or other Feild
in other word each time i generate gerber for a new design it
overrite last one so that may dagerous to screw files ..
or keep one .ppf file for each design that also error prone
(i look for generate the .ppf by report genrator but must have better/simpler way ?)

Click to expand...

Yes, not design fields but if you use a workspace for each design you can set the output folder to be different in each workspace.
This is what is used to prevent you overwriting output files (amongst other things).

T5400 said:

3-) i read a ton of post about vanising via issue and idea to let it whit small section of trace
but did since recent year did have any other solution comming ?
that very annoying since i use lot of via on copper pour and themal pad of QFN
and even fixed it varnish , cannot belive someting so simple as put multi via on a same templace
was not handele right ? (and possibility add free via then add a net to it)

Click to expand...

I do not see a question here however I know what you are referring to.
This had been a problem for many years and AFAIK is under investigation to try and resolve finally however in the mean time there are some utilities that can be used to prevent the issue.
When routing using RMB and "Tidy respects vias" can prevent it happening, also turning off ring removal when its not needed.
Personally I have not seen this happen for many years, recent changes in the data types have helped.

T5400 said:

4-) any way to set placememt goup attribue in sheamtic (used for replicate placement)
on pcb it easy to select part -> attribut editor -> then back anotation in SCH

if try to do same on schematic (select part then attribut editor)
i not find any o the attribue that replicate placement handel ?

Click to expand...

Yes, in schematic create an attribute - perhaps call it "cluster" (the name is not important".
For each placement group give all the symbols in that group the same number as a value in that attribute.
I.E. for group 1 all the symbols get the value 0, for group 2 all the symbols get the value 1.

Save the schematic, ECO update the PCB to the schematic.
When performing a replicate placement use the clustering attribute and select your attribute i.e. "cluster".

HI Matt

thank for reply ,seem that will time to learn how workspace work i not toutch it yet ..

for clusterig attribute i have lot of use attrib
but on pulldown of attribute aviable it very short list
so think my question was more what control the dispaly on that pull down menue ?
and attribut listed on that pull down was not on visible sch side to

did may related to .lib ~ prefix in attribut ?



Best regard
Marc L.

- - - Updated - - -

Hi

so since i like to play whit script i do small scrip that generate batch process .ppf file

so it may interest other user and use a start base ..

this add "Design title" name to prefix to usual gerber name
will need to edit text part for match your color file name ..

Best regard

Hi Marc, in the schematic if an attribute is not already available for you to use then make a new one, this is under "Settings\Attribute Names". Then "Add", choose a name for it, the usage should be symbols and components.

Then it will be available in the replicate function dialogue.

Add macros to your toolbars in scheamtic to change net code bfore you add connection much more efficient...
'Recorded by CADSTAR macros.dll version 6.0
AddConnection
BeginTyping
EditSetFocus 12031
'Macro Stopped
Text "w SIG\r"

You can select groups of nets using the edit net tools if they are named.