hii am learning the concept HDL schematic design.(15.7) until now I used 6 different schematics editors (one editor for 1...60 projects, mostly Altium Designer), but i never had these problems.how can i make all pin numbers to be visible in the concept hdl, without setting them separatelly?in the software manual, they say "after packaging" and "after backannotating"...but i want to see them during I create the design, not after. after its too late to see them.anyway, what is "to package the design"? and how can i backannotate anything if noone started designing the layout, because the schematics is not finished (not even started)?...is it possible to put the first component in the schema, with the pin numbers already visible?the other thing: i have a reference design given in .CSA files, 100 of them. how can I just open them?how can I change a footprint on a component, which is already in the schematics? with a browser, where i can see what i get... for example i want to change a capacitor package to a bigger one..."PATH" is the refdes?
Hi,You need to run the section command.Type "sec" in the command console, then left click your component. pin numbers should appear.Subsequent left clicks with either: remove & replace pin numbers, or step through the available pin numbers for the different sections of the part (in the case where you've drawn a multi-sectioned body, like a single AND gate from a LS00)I haven't tried this, but if you want to section all bodies on a page, tryfind bodiessection xwhere x is the name of the group cadence puts the bodies into.Path is not the refdes, it's a locator used by cadence to identify the body in the schematic. Think of a multi bodied asic. Each body of the ASIC will have a different path, but all bodies will have the same refdes.$location is the refdes.To change the body of the cap, try the edit comand, then navigate to and open the cap body. If you are using a common library, don't move the pins - or you will have a bunch of angry engineers beating on your desk (or maybe on you, it depends how much coffee they've had!! :) ), instead, create a new version of the cap.
Quote: "the bigger thing: i have a reference design given in .CSA files, 100 of them. how can I just open them?"Create a dummy project; all the way to creating a schematic; Save a Page 1Put all the .CSA files in the SCH folderThey will open. :) These are simply the ASCII formatted files for the schematic pages. This is how I supply updated pages to customers. They simply delete the .csb, css and csp files; and save my new .csa files.This is also a way to open older version Concept schematics. Newer versions will open older .csa schematic. I used to do this converting UNIX schematics to Windoze. :)Good day.Mitch
Hi Mitch, Reading from your above post, I have a related question that needed help. I am looking at my design and want to update all the reference designator. For example, like Orcad, I can turn all refdes to ?. How do I do that in DE HDL? This would be a great help. Thanks for the above post, its helpful to me as well. Jason
Use Tools->Global Update->Global Property ChangeThs can be used to change property values across the design, sheet or module - you'll need to change LOCATION and $LOCATION, preserve the source property and reset the value to ?. Make sure that you take a backup - this will affect placement if a brd (PCB) exists.
Hi Andrew, Thank for your reply, I got your reponse on the other thread. May I ask where you are based?, I am based in Taiwan. Just wondering where you are, because it's a strange time for US/Europe to reply at this hour. Thanks again, Jason Huang
Normally based in the UK but in Sweden this week
Cool, Hello from the other side of the world: )