Is there any way of manually adding a component to an Allegro PCB design using PCB Design XL in the same way that you could in OrCad Layout.
I have been able to copy a footprint but the component is unassigned (R*) and I cannot find how to assign it a new part number and to connect nets to it. In Layout, there was a feature that allowed you to add components and manually stitch nets to them.
The impossible we do straight away. Miracles take a little longer.
Yes but it's not advised........ You need at least and XL license (High Speed in 16.5 / 6) and then use Logic - Part Logic. You'll need to enable a user preference to do this. Once done the part will be avaliable to place from the Place - Manually menu (as you would normally). Then use Net Logic to add nets to the newly added part.
In reply to steve:
I have an XL licence. I did add the part to my schematic, but when I imported it, more than half the components got removed, then it complained about part name lengths being too long.
I know it is not advised, but I need to get this PCB finished ASAP and cannot hang around waiting for our own IT to fix these issues. This is using SPB 16.3 by the way.
In reply to tmd63:
Depends on the front end tool (Capture or HDL) but in PCB Editor go to Setup - Design Parameters - Design tab and set the Long Name Size to 255 then import the netlist again.
Thank you Steve,
That has fixed my issue. Althought there were still errors on the devices about pin names and un-named pins. But at least I got my new part in without removing all the other components.