Stats

  • Locked Locked
  • Replies 5
  • Subscribers 164
  • Views 5855
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Reg:Negative Artwork in Allegro

Sakthivel

Hi,

   I am using Allegro PCB Editor. What is the meaning if we set the negative artwork while defining the cross section of layers (through setup-cross section). Is it mean that negative artwork is generated while gerbar file creation or else what ever we see on that layer will not come in  the actual PCB like Orcadlayout?

   Plane layers to be definied negative or postive Artwork? If we define as negative layer (through setup-crosssection)  is it mean that where ever we define the copper, won't come on real PCB and viceversa?

    

Thanks in advance,

 Regards,

Sakthivel

Ucal Fuel Systems.

 

 

  • Khurana

    Yes, when you set layer to be negative in cross-section then the gerbers are "negative" however in Allegro for that plane layer you would see what you get (WYSWYG) i.e. you will see copper for the plane layer in Allegro.

    Regarding plane layers being defined negative or positive I think majority of the designers prefer negative since it reduces the design size.  It does not mean that where you define copper, it won't come on real PCB for reason mentioned above.

  • mcatramb91

    This is not exactly true: "when you set layer to be negative in cross-section then the gerbers are negative"
    Basically, setting the layer to Negative will tell Allegro the way this layer should be treated by the DRC System and how the shapes are to be treated. The Film Control Record for the individual gerber layer controls tell how the layer should be output during Gerber generation "Negative" or "Positive" Image using the Plot Mode setting.

    You can see the effects by adding a dynamic shape on a layer that you defined as "Negative" in the cross section.  You will not see any auto-generated thermal reliefs using traces but you would see crosshairs where vias and pins are connected to the plane.  If you defined flashes for your thermal reliefs in your padstacks along with Flash symbols than you would see the WYSWYG thermals instead of the simple crosshairs at the via and pin locations. Now if you go back into your cross section and change the layer to "Positive" the shape will automatically generate dynamic thermals on the layers driven by your Shape Parameters.  You can even further see the different by adding trace on the layer on top of the dynamic shape which will not automatically void around when set to "Negative" in the cross section but will void around the trace when it is set to "Positive" in the cross section

    Hope this helps,
    Michael Catrambone
    UTStarcom, Inc.

     

  • Khurana

    Sure - you point is well taken.

    When you go to the Film Control tab and select the film then what causes whether Positive or Negative is selected for Plot mode? 

  • mcatramb91

    Normally, the Plot Mode is always set to "Positive" with the only exception being on Negative plane layers so the gerber is generated in a reverse image. (Copper = Clear and Void of Copper = Solid)

    Basically, if there are traces on the layer then the Plot mode will be "Positive" and if you have dedicated power and ground planes which are Negative with Thermal Reliefs which are driven by Padstacks Thermal Flash definitions then its Plot Mode should be "Negative".

    Hope this helps,
    Michael Catrambone
    UTStarcom, Inc.

  • Sakthivel
    Dear Sir,

    I am Sakthivel working as an Embedded Hardware Engineer. Since I am new to PCB Design I thought of asking some few basic questions. We are not following any standard for design of PCB’s (Since we don’t know what standard to follow). Is it necessary to follow any standards for PCB Design? I came across IPC Standard (Institute for packaging circuits). Shall we follow these standards for PCB Design for our PCB Design? How much will be the cost of these standards? How can I get these standards?

    Thanks & Regards,

    S.Sakthivel,
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. 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. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.