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.
The 16.6 Allegro RF PCB application has many new enhancements.
I’ll cover a few over the next several weeks. Here are some major autoplace related enhancements:
Read on for more details …
Autoplace is a very important step for RF layout after the schematic is transferred to PCB layout. The system will automatically create groups based on connectivity during the autoplace process. This will result in many groups in autoplace and it’s difficult to find the proper groups to do autoplace. Designers like to define groups in the schematic based on functions such as LNA, pre-amplifier and so on and then select the proper groups to start autoplace. In 16.6, we’ve added some new commands in DEHDL to support grouping, such as add group, disband group, display group and so on. In this case, designers can easily control the groups for autoplace. The detailed commands are:
All these commands are only available in the DEHDL pre-selection mode.When you transfer the schematic to layout and launch autoplace, you will see the groups are classified differently, the group names added in schematic are reflected in the autoplace form: You can use the Group filter to easily find/locate some specific groups to do autoplace.
RF Grouping in the Front End (DEHDL)
To use the grouping functionality in the schematic, you need to select Tools->Options and check the “Enable Pre-select Mode.” You will see the RF PCB menu as follows:
If you check “Enable Windows Mode” as well, then Import IFF… item will not be available under the RF-PCB menu. You can find it from File->Import->Import IFF…->RF-PCB.
You need to first select some RF components (or non-RF components) and then click RF-PCB->RF Group->Add Group. The following dialog will pop up: You can enter a new group name or select an existing group from the drop-down list. If the existing group includes elements outside the current page, you need to select Module radio option. You can only select the components in current page to add to a group.
Select a wire or multiple wires and then click RF-PCB->RF Group->Add Split. The RFSPLIT property will be attached to the wires selected. You can’t select wires crossing pages to add split. That means you can only select the wires in the current page for this command.For example, in the schematic, two wires are attached with the RFSPLIT property as following: There will be three logic groups in the layout for autoplace even though they are actually connected together logically:Disband
Click RF-PCB->RF Group->Disband. The following dialog will appear: All available groups will be listed in the drop-down list. Select a group and select the proper scope and then Apply to disband the group. The RFGROUP property will be removed from each component of the group.
Select one or more components with the RFGROUP property attached or one or more wires with the RFSPLIT attached and then click RF-PCB->RF Group->Exclude. The property will be removed for the selected objects. This command also works for the current page objects only.Display Group
Click RF-PCB->RF Group->Display Group. The following dialog will appear: You can display one group from the drop-down list or all groups by selecting All from the drop-down list. To display a group including elements in other pages, you can select Module radio option. Click Apply or OK. All components within the selected groups will be listed in the command line if the module option is selected, and the components of the selected groups will be highlighted in the current page.Display Split
Click RF-PCB->RF Group->Display Split. The following dialog will appear: OK to highlight the wires with the RFSPLIT property in the current page. To get the description of each wire with the RFSPLIT property within the current page, select Page option. To get the description of each wire with the RFSPLIT property in the whole design, select Module option.
Enhancements in Back End (Allegro PCB Editor)
In layout, launch RF-PCB->Autoplace. The dialog will appear:All components will be classified into different logic groups. Each logic group will have a name with the prefix “_rfGroup”. If you have already defined a group in schematic (for example ABC), then this name will be the name for a real physical group in layout. This name will be attached following the logic name within brackets such as _rfGroup1(ABC).Some other enhancements for autoplace are:• Add a new check box “Ignore FIXED property”• A new mark “A” for the groups just completed autoplace• A filter to find/locate a group• Ratsnests display during autoplace• Moving clearances• Performance enhancements If you check the “Ignore FIXED property” option, then a fixed component can be moved as well during the autoplace.There are two kinds of marks for the groups. A group with a “P” mark means this group is already placed into canvas before the autoplace command launched. A group with an “A” mark (green color) means this group completed the autoplace in the current session. A group without any marks means this group is still unplaced and you may need to do autoplace for it.The autoplace is enhanced to show the ratsnests while the dynamic path is attached to your mouse during the autoplace process. This makes it is easy for you to place the group to the proper location: Another enhancement is to support the clearance moving as well for the autoplace--for example, after completing the autoplace for a logical group and then adding the clearances for the components within the group. If you redo the autoplace and move to a different location to place the group, the clearances will be moved as well. Before that, the clearances will not go with the RF components: Please share your experiences using these new capabilities.
Jerry “GenPart” Grzenia