SPICE simulator: could save a bit of time, but there are simulators elsewhere
Yes there are simulators elsewhere but then you have to draw things multiple times in different tools. Better to draw it once surely?
PCB layout software has new modular design blocks: already in 7.7; is the implementation any better? Normally I import the .brd to replicate layouts.
They've basically wrapped it up in the UI and added a dbl file containing the portions of the sch/brd. You can create it from a small section of an existing design too.
Schematic rule check: already in ERC; anything new or helpful?
Nothing new in the ERC really.
Schematic to PCB synchronization: fundamental to EAGLE, nothing new here
Yep, nothing new here.
PCB layout editor: routing engine looks interesting, but as I said, I've learned how to work with 45° corners, careful rip-up/dragging of traces etc.
The new move tool with preserve angles is SO much better than in earlier versions of EAGLE. It's actually a huge productivity increase for me.
PCB object alignment: snap to grid, changing the grid size dynamically is enough for me
There are actually some additional alignment tools too but honestly I don't use them much because I use grids a lot.
Obstacle avoidance PCB routing: as above
It can be useful but it's not grid aware so tends to leave things off grid which I then have to go clean up. It's useful for quickly seeing routing options.
PCB routing: as above
There are actually quite a few new routing tools, the most notable of these being push and shove which can be hugely helpful when you need to get some traces through on a congested board. Another additional routing mode is loop removal which makes rerouting traces a different way a lot quicker. There are also a whole bunch of modes associated with the ripup tool now too which can be very helpful at times.
Simpler selection and editing: old way works okay
Old way works better. Fortunately you can still use the old way by turning the "Group command default on" setting off.
High-speed design: is diff pair any better than before?
Not yet but hopefully this is something they'll improve upon soon.
Design rule checking (DRC): old hat, unless there are new, useful checks?
Well, there are some new checks and some additional settings to help determine what gets checked but the biggest changes to the DRC are:
1) Live DRC. It's running all the time so you can see violations as you are routing and deal with them as they occur rather than only find out when you've manually run it at some later point. It's actually much better than it sounds and I find it incredibly useful.
2) The DRC results window has been improved so you can find and see the errors you wish to deal with more easily.
PCB library content: I mostly make my own library parts and I'd rather not rely on online stuff. Trust issues with parts means I would probably have to consult the datasheet anyway.
Yep you should always make your own stuff and if you do use anything else from a 3rd party it needs thoroughly checking. The libraries which are supplied aren't improved and I don't use them. However, there is now an IPC package generator which creates quite a lot of standard package types along with 3D models to go with them.
They have also introduced "Managed Libraries" but these have some usability and workflow issues. For the most part the regular libraries are better but in order to fully utilize the integration with Fusion360 you do really need at least one managed library for dealing with mapping STEP models to footprints.
PCB component 3D model: could be handy but I can export to DXF and this is usually enough for 3D CAD
Being able to create a proper 3D model of your board and seamlessly go between ECAD and MCAD in either direction is quite a big bonus if you are designing anything with any significant mechanical design challenges. You can move parts and alter the PCB outline in Fusion360 and push them back to EAGLE so it's much closer integration than just exporting a static model from ECAD and loading it into MCAD.
Complete component: I can copy an existing component footprint, even though it has a strange workflow. Reusing existing libraries carries the same risk as before.
Yes, there are no real changes here.
Link component to supplier: with BOM ulp and our own tools we have this covered already
I've never used this part at all, I do my own thing for BOM's etc. I think the DesignLink stuff came in v7 under Farnell?
Online PCB community: CAM processor and choose your own board house
Yes.
Fusion 360 Integration: as above
It's actually quite useful. See above!
User language programs (ULPs): very useful but nothing new
Yes there haven't been any improvements in ULP really.
BGA fanout: personally I don't work with BGAs. I remember that the integration was a bit buggy at the start, is it better now?
The BGA fanout isn't useful. It was one of the first things they did early in v8 and hasn't been improved at all since. I do a lot of BGA designs and I always end up just routing them out myself. This is now part of a larger fanout tool which provides better support for fanning out components in general.
As above, the new routing and auto net/label placement for schematics look quite neat. I just think at the moment that this is not worth some 700€ per year in perpetuity on a software model I don't really support. If I had the option of a one-time permanent licence now that I can actually see what I am paying for in advance, I might consider it.
There are other improvements too which aren't covered in the above list. In the schematic editor busses now have good support in the UI. Previously you had to explicitly write the bus strings to create them and I wrote a ULP to add some UI functionality to this previously, but now there is a proper UI built it which does make creating and managing busses a lot better.
In the board you now have true bottom side view which is an actual flip of the view and not the design editing mirror.ulp which was provided previously. You also have single layer mode so all but your currently active layer are greyed out so you can get a clear view of where you are routing but still see what is of interest on other layers too.
It's up to you whether you feel €700/year is too much but at least they are now actually providing the updates people had been asking for which could never have been achieved with the old CADSoft model as they just couldn't sustain the amount of engineering required. When the subscription was first announced there was a lot of anger and an assumption that it was just a money grab and nothing would come of EAGLE. I think they've definitely shown they're willing to put a significant investment into the development of EAGLE now so I think we'll continue to get significant improvements with future releases so the subscription model isn't an issue for me, I know it goes to paying for software development and I will see the results in time.
Best Regards,
Rachael