I have a layout which is partially complete in VXL. The schematic got changed and I have few more instances to place in each layout. I see that this can be done using "Create ~> pick from schematic" and then selecting the instances.
Is there a way to replicate this process using SKILL , so that I dont have to open each layout to do this. I already have a routine that gives me the list of instances to be placed in each layout.
I tried to instantiate these using dbCreateInst() but then I dont get the flyline connectivity between the inital instances and the new one. Can someone please help ?
To get flyline connectivity, you will need to create nets and instTerms. Let's say you have a simple cell that consists of two instances I1 and I2. Each instance has a pin called IN and a pin called OUT. The OUT pin of instance I1 connects to the IN pin of I2 as a net named NET1. At this point, you have written the Skill code that creates the instances I1 and I2. You now need to create a net in the cell called NET1. You can then create instance terminals (instTerms) for I1 pin OUT and I2 pin IN that connect to NET1.
cv=geGetEditCellView()i1 = dbCreateInstByMasterName(cv "mylib" "myinv" "layout" "|I1" 0:0 "R0")i2 = dbCreateInstByMasterName(cv "mylib" "myinv" "layout" "|I2" 10:0 "R0")i1Out = dbFindTermByName(i1~>master "OUT")i2In = dbFindTermByName(i2~>master "IN")net1 = dbCreateNet(cv "NET1")it1 = dbCreateInstTerm(net1 i1 i1Out)it2 = dbCreateInstTerm(net1 i2 i2In)
I haven't run the above code but it should be close enough to working order. The instTerms describe how the nets connect to the instances so you can get flight lines. If you create top level pins using leCreatePin, it will create a net and a terminal and the pin shape all in the same command (without the need of using dbCreateNet, dbCreateTerm or dbCreatePin). You can find out more about these functions in the Cadence Design Framework II SKILL Functions Reference.
In reply to dmay:
Thanks for you reply. I get the basic Idea how to do it from you post, but then for each instance pin, I will have to do this, means look at schematic, make a list of list of pin connections and nets and then wrap that around on the above mentioned code. But is there a way to get SKILL equivalent of " Pick From Schematic" , like for genFromSource, I found that we have "lxGenFromSource" but then it doesnt take into cosideration the placement and routing already existing in the block.
In reply to Kaggarwa:
The only command I am aware of is an interactive command: lxHiCreateInstFromSch()Running this command is no different from invoking it from the Cadence menu. Putting the above commands in a procedure should not be too difficult unless you have parasitic devices in the schematic that you want to short through. If you look at instances in the schematic, you can see that they all already have instTerms, so you just need to create the layout equivalents.
From an instance in the schematic, you can get everything you need:
Select an instance in the schematic:inst = css()foreach(it inst~>instTerms printf("Inst Name: %s Term name: %s Net Name %s\n" inst~>name it~>term~>name it~>net~>name))
Thanks for your guidelines.Looking inside lxHi commands, I came across another fucntion of UpdateComponentsAndNets. This is again interactive though , but now atleast I place all my instances using Skill and just do this update command and it attaches all the terms with proper net names etc and gives me the necessary connectivity flyline too. it seems there is no way currenty to run these commands in batch mode.