Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
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 :-)
In reply to SKILLBILL:
are you using chrome, I find chrome behaving like this
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
In reply to vramanan:
the example file
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
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
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
In reply to Ejlersen:
Turns out I could do a remote session and get access to PCB Editor.
In Release 16.3 the syntax is
setwindow pcbtrapsize 205etcheditdlib setwindow form.dlibFORM 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 pcbetchedit
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 ?
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.
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.
In reply to AmyZhang:
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.