Questions about using Cadence Allegro

[buenos]

hi

i have some questions about using cadence allegro. and i will have more later.

Q:

- in the Pad Designer (padstack editor), i can sppecify only one diameter for a circle thermal relief for positive planes. But which is that parameter? normally a thermal relief is a pad in a bigger antipad, and there are 2 crossed traces. all of these have dimensions, but which (single) one is what we provide? and what about the other parameters, like the crossed-trace width? where do we specify them?

-how to specify a thermal relief, to get a direct/solid connection to the planes, instead of a real thermal relief? how on positive, and on negative planes?

-in drawing a component footprint. i want to put a pin. i pressed the layout>pins, then i wanted to browse for a padstack, but after pressing the browse button, nothing happens. I can not place any f***** pin for a footprint. what to do?

-i am doing component manual placement. I set the toplayer pads to be red. i switched off all the not important classes/subclasses. but all the component pins look light blue, with very thin 45 degrees red lines. If I move the components, their pins look red. what is it?

 

[buenos]

allegro fill pads

-how to move a package designator, when the package itself stays? like in Altium designer. for an individual component, not for all with the same footprint

 

[richardLC]

allegro cis commands

looks you're using allegro just at beginning. , you need some time to get used to it, good luck.

- in the Pad Designer (padstack editor), i can sppecify only one diameter for a circle thermal relief for positive planes. But which is that parameter? normally a thermal relief is a pad in a bigger antipad, and there are 2 crossed traces. all of these have dimensions, but which (single) one is what we provide? and what about the other parameters, like the crossed-trace width? where do we specify them?

A: if you don't use shape/flash, when you place the components in the board, you can assign different with for the 2/4/8 crossed traces( we call them spoke width), but if you decide to use flash/shape in neg. plane, you only can use what you had designed in your pad-editor. by the now technology, I strongly suggest you use positive plane, WYSIWYG, more flexible control ... , size of gerber file is not a big issue now.

-how to specify a thermal relief, to get a direct/solid connection to the planes, instead of a real thermal relief? how on positive, and on negative planes?

A: same as above, in your shape parameter, chose which style you want to connect to plane, diag/cross/full/8way/best fit..... you name it, a lot.

-in drawing a component footprint. i want to put a pin. i pressed the layout>pins, then i wanted to browse for a padstack, but after pressing the browse button, nothing happens. I can not place any f***** pin for a footprint. what to do?

A: this is a very frequently question for newbie, , check your Setup->User preference...->design path->padpath..... add all the path where you saved your pads.

-i am doing component manual placement. I set the toplayer pads to be red. i switched off all the not important classes/subclasses. but all the component pins look light blue, with very thin 45 degrees red lines. If I move the components, their pins look red. what is it?

A: one components doesn't mean they only have "physical-copper-pad" on it, soldermask, anti-stuff, pastemask, pinnum, top/inner/bottom,.... make sure all the layers you don't to see are closed(you may use ALL-invisible then visible something after click color button in toolbar), meanwhile check your pad-fill mode and shape fill type (in setup), and something related with hilight (net,symbol,pins,functions.).... normally at your right hand's Options panel.

sorry for my not proper english, I am not a english speak person when I back home

 

[buenos]

allegro how to move ref des

ok

thankx the answers.

there are padstacks in the folders specified in the padpath variable. even then, no browsing window appears when i want to place a pin. so? how to make it work?

 

[buenos]

allegro can not see pad

- the cross select doesnt work for me with the capture cis. i enabled the intertool communications in the CIS. what else to set up?

-how to move a component designator for one component (not in the library footprint, with all substances) a littlebit away on the PCB board design?

Added after 3 hours 11 minutes:

how to change net assigment to an object: shape, or line... ? in a manual of allegro 14.x, they say: Edit>Change_Net(Name) . I use allegro 15.7, and this menu doesnt exist. there is a change menu, but if i use it, there is no popup window to select a net, but it says "object already matching control panel settings"

 

[richardLC]

allegro reassign net to shape

ok
thankx the answers.
there are padstacks in the folders specified in the padpath variable. even then, no browsing window appears when i want to place a pin. so? how to make it work?

if your padstack is correct(same as shape/flash if your padstack need it), you should have it available in your Symbol design, notice that you can't place pin in BOARD design.

Added after 8 minutes:

- the cross select doesnt work for me with the capture cis. i enabled the intertool communications in the CIS. what else to set up?

-how to move a component designator for one component (not in the library footprint, with all substances) a littlebit away on the PCB board design?

Added after 3 hours 11 minutes:

how to change net assigment to an object: shape, or line... ? in a manual of allegro 14.x, they say: Edit>Change_Net(Name) . I use allegro 15.7, and this menu doesnt exist. there is a change menu, but if i use it, there is no popup window to select a net, but it says "object already matching control panel settings"

you don't need to move reference (you mean C1,C2,U5,...?), if you don't need it. you just delete it! when you want it back, re-update the symbol. then you get everything back.

line doesn't have net on it, the "line" (with net) we call them trace/cline.

select shape, then you will find you can assign that to any net (Option panel in your right hand). I never do this way through menu, so I don't know if something change or not from menu for this net assignment. another thing is even you assign a net to a shape, you may need to check how other etch connect to this shape, in some condition, you may see pad still not connect with the shape(because of the not proper connect type).

 

[buenos]

allegro + moving reference designators

thanx

i can see pads in other cases, like constraints-settings, or with component-wizard. but not in manual drawing of components. if i click on a browse button, there should open a browsing window, even if it shows: no elements found. but for me, nothing appears.

i need the reference designators. i worked always wih altium, and it was a good feature that i could move the refdes without moving the component. i moved reftdes to locations, where there is no component-pin... and make more tight and effective component placement. but now with allegro, i have to put components away from each other, otherwise the refdes overlaps with the neighbor-components's pins. or... is ther a way to move it?

 

[majnoon]

cadence allegro questions

I was reading your questions and hoping that you will finally get the answers either by yourself or others will tell you...
Richard has provided some good replies.

My suggestion is STOP thinking what ever tool you were using before.
Is hard not to compare but try to stop bringing other tools into new one you know what I mean?...
Now to one of your questions, Reference Designators. First what are they?
Use "i" button and get info they are TEXT! now use ample and I mean it really use Control Menu in Allegro select your command in this case MOVE and in Control menu select only TEXT and Voila it moves! Same for everything else.
Be happy you are using one of the best tool available out there.

Good Luck,

M

 

[buenos]

rotate component allegro

thanx.

this text-trick seems obvious afterwords already, but i couldnt figure it out by myself.

i still have the problem with the padstack-select browser in the footprint-editor

 

[majnoon]

rotating shape in allegro

I am sorry you need to be more clear on your question.
Maybe you can post a pic?

Regards,

M

 

[buenos]

set command in allegro ini file

here is a video, not a picture:
(about the not appearing browsing window)

 

[majnoon]

allegro thermal relief flash

First check your pads path.

In setup>user preference>design_path
make sure pads are pointed to directory that you have your pad stacks.

Same thing for psmpath.

This should fix it.

Let us know.

M

 

[sigint]

allegro altium rotate

If all else fails, Allegro can be touchy with path hierarchy, dump all your symbols and pads into the same directory as the .brd file - thus is not great practice but it may get you moving - remember - with everything you choose what you want to do, what kind of element - then select - the logic is backwards from a lot of tools, the box on the right hand is key for most things.

SiGiNT

 

[buenos]

allegro 15.7 rotate symbol

i have all the padstacks copied to the project folder, and to the 3 folders, specified in the padstack. i am saying again, that the problem is not an empty browser window, but the browser window doesnt even open.

something else:
how can i extract a topology of some traces together post-layout from a pcb, to make crosstalk simulation in the sig.explorer ?

Added after 1 hours 20 minutes:

how can i extract the topology of a diffpair to the sigxp?
if i try it, it shows a single net, not a pair.
i tried in the same way as its in a tutorial. one difference: there are no differentiel-ibis models, but the diffpairs are made in the logic>assign_differential_pair

i tried this way:
-in the constraint manager, i clicked on a diffpair name at the net>routing>diffpair and rightmouseclick>sigxp
-in the analyze>si_emi_sim>preferences the differential_extraction_mode=on

Added after 20 minutes:

how to add an ibis model file to a component? i dont want to specify the ibis details, just i download the single ibis file for a component from the internet, and i want to use it.

Added after 2 hours 46 minutes:

how can i do power integrity analysis? please detailed. (impedance at given points vs freq, or at a whole surface at a given freq, ssn distribution on the surface)

 

[buenos]

how set psmpath cadence allegro

what is a bus simulation? why it doesnt work? (error message: signal model doesnt have model selector...)

 

[buenos]

move and spin allegro

is it possible to rotate a component by 90deg during movment, by a keyboard pressing? (without clicking right, then menu, spin then ...)

 

[dsPIC24F]

allegro 15.7 control menu help

That's really a lot staff to learn. Is it always so hard to get started?

 

[richardLC]

allegro cline change net

is it possible to rotate a component by 90deg during movment, by a keyboard pressing? (without clicking right, then menu, spin then ...)

Sure it's possible,
for example, if you want use Ctrl-R to rotate your component, just add "alias ~R rotate" in your "allegro.ilinit" file or command line or somewhere else.

from the menu "Tools->Utilities->Keyboard command..." you may find more informations.

 

[buenos]

capture-cis no-footprint-selected

thanx.

in the altium, if i press space, the component already rotates left by 90deg. if i want to rotate right by 90, i have to press 3 times, but even then the whole thing takes 0.1-0.5seconds. with the allegro, if i want to rotate, then i have to move the cursor away from the components, turn around, then the component moves away a littlebit and I have to move it back to the original location... it takes much more than 0.1-0.5secs, around 1-2secs. but if there are thousands of components, it can be weeks of extra time in design.

so, is it possible to use rotate in allegro, like in altium? (fixed rotate left by 90deg, immediately after i pressed a button)

 

[buenos]

thermal reliefs on positive planes

in the sigwave window, there are results like:
boardfile_component_pin
boardfile_component_pini
boardfile_component_pin_buffdly
boardfile_component_pin_buffdlyi

whats are these?

Added after 35 minutes:

whats are the meanings of the values of the crosstalk timing windows?
like someone prowides this: XTALK_SENSITIVE_TIME= 150-175, 400, 450-475
what does it mean? how do they measure the time? what is 150? phase degree? picosecons? what is 0?