skill program to create shape symbol 

Hi

Attached, find a small utility to help creating rectangular shapes with rounded corners for shape symbols to be used inside a pad

Usage: File, New, Shape symbol

Run the program "ns_spad"

Add width(x), height(y) and a radius in the dialog shown

Hit run to create the shape.

Have fun :-)

Ole

 Hi Skillbill

are you using chrome, I find chrome behaving like this

Use Firefox

Seach Google or the forum for FPM (Foot Print Make)

It has all the tools you need to create symbols and padstacks

regarding surface mount pads yes I see there is a need for a utility to  quickly create padstacks

 I will investigate on this and let you know my findings

regards

Venkata

 Hi Skillbill

the example file 

%cdsroot%/share/pcb/examples/skill/dbcreate/pad.il

will create 2 pad files 

MY_PAD and SMT_PAD

it will not create a physical PAD file but will create the pad definition inside the allegro database

to see them go to Tools-> Padstack->Modify Design Padstack

Now you should see those definitions

you could either save them by Editing and invoking the padstack editor or File->Export->libraries and chooseonly padstack

as mentioned in the help doc this will not work in the symbol editor

I can see that using this you could create a quick SMT pad on the fly and replace an existing pad

regards

Venkata

Hi vramanan

This is great. Wonderfull. I made it, thx to your idea vramanan. I have created padstack.

You are 100% right. With the help of axlDBCreatePadStack function padstack is virtualy created in allegro database.

Export of the padstack allso works.

Right now I am working on a way to automaticaly export this pad.

Some time ago mr Ejlersen showed me a way to fill forms that pop up in allegro.

Back then i was filling form that poped after nctape_full command

and i used this code

tmp_file = axlDMOpenFile("ALLEGRO_SCRIPT", "tmp", "w")
      fprintf(tmp_file "scriptmode +i +n +w +c\n")
      fprintf(tmp_file "setwindow pcb\n")
      fprintf(tmp_file "nctape_full\n")
      fprintf(tmp_file "setwindow form.nc_drill\n")
      fprintf(tmp_file "FORM nc_drill tape_name NC_Drill_%s.drl\n" filename)
      fprintf(tmp_file "FORM nc_drill auto_tool_select YES\n")
     fprintf(tmp_file "FORM nc_drill separate_tapes NO\n")
      fprintf(tmp_file "FORM nc_drill repeat_codes YES\n")
      fprintf(tmp_file "FORM nc_drill optimize YES\n")
      fprintf(tmp_file "FORM nc_drill execute\n")
      fprintf(tmp_file "FORM nc_drill close\n")
      fprintf(tmp_file "setwindow pcb\n")
      axlDMClose(tmp_file)
      axlShell("replay tmp")
      if( isFile( "tmp.scr") then deleteFile("tmp.scr"))
      printf("NC Drill created succesfully\n")

now i tried to modify it a little but i dont know the name of the form dlib opens.

This is what I have tried:

tmp_file = axlDMOpenFile("ALLEGRO_SCRIPT", "tmp", "w")
         fprintf(tmp_file "scriptmode +i +n +w +c\n")
         fprintf(tmp_file "setwindow pcb\n")
         fprintf(tmp_file "dlib\n")    
         fprintf(tmp_file "setwindow form.export_libraries\n") ; this is where i am wrong forms name aint form.export_libraries
         fprintf(tmp_file "FORM export_libraries mechanical_symbols NO\n") ;checkbox set to NO but i am not sure to the name of those checkboxes. I used the names i found in help under "dlib"
         fprintf(tmp_file "FORM export_libraries package_symbols NO\n")
         fprintf(tmp_file "FORM export_libraries format_symbols NO\n")
         fprintf(tmp_file "FORM export_libraries shape_and_flash_symbols NO\n")
         fprintf(tmp_file "FORM export_libraries device_files NO\n")
         fprintf(tmp_file "FORM export_libraries padstacks YES\n")
         fprintf(tmp_file "FORM export_libraries no_library_dependencies NO\n")
         fprintf(tmp_file "FORM export_libraries execute\n")
         fprintf(tmp_file "FORM export_libraries close\n")
         fprintf(tmp_file "setwindow pcb\n")
         axlDMClose(tmp_file)
         axlShell("replay tmp")
        if( isFile( "tmp.scr") then deleteFile("tmp.scr"))

it doesnt work...tho..

If you have a clue of those params pls tell me. I feel i am so close :)

Damn you are good vramanan :D

I am realy happy and impressed

Have a nice day

Hi SkillBill

I'm not sitting in front of PCB Editor at the moment, but when I have difficulties with skill writing script files I normally do the following

1. Record a new script where I do whatever I want to do.

2. Carefully check that all my fprintf lines are correct - it only takes a very small spelling or syntax error to fail. Sometimes I even redo the script write commands in my skill program.

3. Comment out the line "if( isFile( "tmp.scr") then deleteFile("tmp.scr"))" because then I can try running the script "tmp.scr" manually or do a file compare with my previously recorded script.

4.  Remove +i +n +w +c from the line "fprintf(tmp_file "scriptmode +i +n +w +c\n")" since that may give better warnings as to what the issue could be.

Hope this helps

Ole

Hi

Turns out I could do a remote session and get access to PCB Editor.

In Release 16.3 the syntax is

setwindow pcb
trapsize 205
etchedit
dlib
setwindow form.dlib
FORM dlib mechanical NO
FORM dlib package NO
FORM dlib format NO
FORM dlib shape NO
FORM dlib device NO
FORM dlib pad NO
FORM dlib pad YES
FORM dlib nodepend YES
FORM dlib execute 
FORM dlib cancel 
setwindow pcb
etchedit

Best regards

Ole

Hi Ejlersen

I want to thank you very much.

You have shown me a way to aquire very important information regarding forms inside allegro.

I am really grateful. This is huge for me.

Many many thanks. Have a nice day Ejlersen.

PS. One more thing. I dont know what "trapsize 205" does ?

Hi

Thanks for the kind words. I usually just cut out the trapsize part of my scripts, the online helps says the following about trapsize.

In Allegro-generated scripts, the tool automatically adds a "trapsize <value>" at the start of a script, after every change in zoom factor, and when opening new databases. If you generate scripts manually, place a "trapsize 0" at the start of a script to ensure that it replays independently of a design's zoom level.

The value, in design units, describes the trap box size where to find objects when an object pick is encountered in a script. A value of 0 requires a pick on an object.

Best regards

Ole

hi,Ejlersen,

the ns_spad skill is useful,but can  it add to the menu by modify the allegro.men?

when open the .brd file,it display in the pull-down menu  which i added,but it disable because "program only runs on shape symbols",

but when i make a new  shape symbol file, the menu that  i added  disappear. i shoud imput "ns_spad" in command line.

  Is there a way to add the skill to the menu?

sorry for my poor English.

Thanks!

Hi

allegro.men controls the menu inside PCB Editor when you work on .brd files.

For .dra files you need to change pcb_symbol.men instead.

Best regards

Ole