I don't think so. I believe PADS only supports negatives for a full plane. If you want to split the plane you have to switch from 'CAM Plane' to 'Split/Mixed' and work with a positive image.
You are right, a cam plane by definition is made from a negative image photoplot, but the assignment dictates how the gerbers are made.
On a cam plane, you have to create the split yourself. Draw a 50 mil line along the board outline to back the plane edge 25 mils from the edge. Draw a 20 mil line across the board to define the split. Usually, your component padstack has a slightly larger diameter pad assigned to a layer specifically to use on a cam plane. This diameter pad also defines the outside diameter of your thermal pads. When you create a cam plane photoplot, Pads simply swaps out the clearance pad with a thermal pad if the assigned net appears on that pin. The problem with cam planes is there is no way to check the plane connectivity in layout since there is no electrical feature to check against. If you put your split line in the wrong place, you could short the planes, or apply the plane net to the wrong pins. Only using a IPC net check on the gerbers would reveal this type of error. If I were working on this design, I would convert the cam plane to a split mixed plane first thing. If the plane was already split, I would set my split gap to equal the line width used to split the cam plane and use the line as reference when I split the planes, then delete the line. Aside from being a carryover to days when photoplotter file size, photoplotter time and storage space was critical, I do not know of any good reason to use cam planes.
Follow up- You can check the cam plane by coloring the pads based on the net name and then visually looking over the layer prior to creating the gerbers, but this approach is all up to you. Shut off all layers except the cam layer. Set the cam layer pad color to dark blue, then in View, Nets, set your two plane nets to have bright, but distinctively different colors like bright green and bright red. Make sure you have the plane layer selected and display current layer last is set to ON. It is still far faster and less error prone to let the system check this.
A few notes:
CAM Plane outputs will use Layer 25 thermal and antipad definitions, you do not need to accept autogenerated pads.
Negative image planes DO have an advantage over positive image planes. Due to processing differences, the spacing between open areas can be consistently smaller using negative process material. This allows more complete coverage and fewer disruption sin signal return paths.
It's not a bad idea to do an IPC netlist test on your gerber files anyway.
If you talk to your fab vendors, you may be surprised to hear many still prefer negative planes.
Thanks for your reply
i like to thanks for Pete and dcox.right now i am working on another project.i will be come across after 2 days.i will work out and let u know
Hi Pete. I understand your comments, but I disagree with your findings.
Let's look at some numbers using a standard dip 14 footprint. The assumption is the footprint uses a .060 round pad with a .037 finished hole. Pads will add .005 to the hole size and work with a .042 dia drilled hole for spacing purposes. Trace widths are .008 wih a .007 space. The assumption for an anti-pad is .085 dia assigned to layer 25 which is saved with the footprint in the library. The .085 is selected to support the size of the thermal, should the plane net tie to one of the pins. Design rules sets spacing at .010 gap for copper and drills.
Standard copper flood retains the .060 pad, backs the copper .010 away from it, yielding .020 wide copper webbing between the pins, (.100 - .060 - .010 -.010) certainly a sufficient coverage to provide reference for a single .005-.008 wide trace.
A cam plane will utilize the .085 anti-pad and give us .015 wide copper between pins. This is less, but still enough for a single trace.
A split mixed plane will remove the pad and back the copper away from the .042 drilled hole and give us .038 wide copper between pins (.100 - .042 -.010 - .010) which is much better if you run two .008 traces between pads.
So, if you intend to run two traces between pads, your copper edge to edge dimension is .023 (.008 + .008 + .007). Neither of the first two planes provide adequate reference copper for this. Running two .005 wide traces with a .005 gap barely works with .020 webbing, but not .015. On top of that, the .085 pad is static and can only be changed by modifying the decals. When creating apertures for cam planes, Pads has a built in algorithm that assigns 75% of the anti pad size for the pad area and 12.5% for each moat. .085 is about as small as you can get (.042 drill + (+/- .004 location tolerance) + (+/- .005 drill walkage) = .060 and add .004 for minimum ipc annular ring = .064 then add 33% for the moat = .0853
I add drawing outlines and assign numbers to all my artwork sets and create pdf files of the gerber documents. My engineers have access to read only Pads licenses and are very pro active when reviewing the designs. They work with a WYSIWYG attitude and like to be able to evaluate plane coverage visually. Fab houses have enough cam work to do as it is without adding more.
All those numbers do not take into account 8 mil vias with 20 mil pads on a 5 mil grid lined up to change layers on a 32 bit bus. Now you have a nice, long slot in your GND plane. Put a 1000 or so vias on that plane, the extra web between vias is welcome.
And it's actually LESS work for the fab house if you give them a negative image plane. They generally stock both positive and negative image photoresist. No consideration required for many thousand draws. Flash some thermals and be done.
I'm not telling anyone they have to use CAM planes, or they are wrong for not using them. I'm simply pointing out some advantages. CAM planes are often misunderstood by people who were not designing boards back when they were the only option.