I suggest you try PCB Elegance.
I found that it crashed frequently when messing around with the PC mobo example. I traced it down to some function being called with a null pointer. I never did pursue it far enough to fix it though.
It was a while ago, but I did make a list of notes about it, which I list here in case it helps:
PCB Elegance 3.50
1. Full version now available without cost. The included gerber viewer,
VIEWPLOT 2.0, however needs to be purchased and unlocked with a dongle
for all of VIEWPLOT's features to be available. Can view, but no
editing and saving.
2. No Blind/buried vias.
3. Modes are confusing.
4. No fine grained clearances. (i.e. all combinations of pad, via,
trace, and layer.)
5. Schematic symbol creation allows for 20 pins at a time, but
pasting in pinnames works. The pinname text, however, is not
tied to the pin, so it is possible to make a mistake if you are
no careful when editing the component during creation.
6. Only 3 grid fixed choices in schematic editor and symbol editor. This
makes it difficult to do fancy graphics. Can use scaling, but stuff can't
be brought back on the grid when scaling to final size. It moves in
the current grid increments, just displaced from the current grid.
7. Layers are opaque. Plane layers are negative so are transparent.
Area fills on plane layers are not transparent, but are painted first,
so that signal layers are not obscured.
8. Can't draw on plane layers except for area fills.
9. Can display properties of things, but can't edit them there.
10. Crashes in the pcb editor, especially when the pc motherboard example
is open and dragging traces or panning.
11. Difficult or maybe not possible to insert a vertex in an existing trace.
"drag one trace" sometimes drags after clicking. Other times, it just
highlights. It gets into the highlighting mode after choosing
right-click->escape. The esc key will not do it. After highlight,
right-click->drag must be selected to get into drag. "d" shortcut does
not work. Or you must go into some other mode and reenter drag trace
mode.
12. Need to highlight something before selecting info command, but you must
be in the right mode to select something and the right mode depends on
the something. (Hover ballons always work on visible objects.)
Info displays a table which includes the one or more items selected.
Info does not work for traces.
13. Drag trace does not work consistently. Erratic at times.
14. Can't insert a vertex, which can be useful before a drag. And dragging
does not insert any vertexes. Therefore, it is not possible to drag
a straight trace that connects two vias, for example. But route net
can be used to modify a trace that has a network assigned.
15. Right-click->"Other menus"->whatever changes modes (aka menus), but does
not update button tiles on the screen, so they get temporarily out of
sync with each other.
16. No permanent display of pin numbers or net names, but hovering shows
properties of vias and traces.
17. No choice of font. Vector only. But schematic can create pdf with
searchable text. Apparently uses courier font when making pdf. It's
nice to not have to worry about it, but the screen appearance can be
different than the print appearance. (slashed zero on screen, no
slash on print, for example.)
18. No net classes, but it is easy to apply class-like attributes (clearance,
trace width, via) to individual nets.
19. No easy way to get a report of board statistics.
20. Stippling (great for color blind people.) 15 predefined patterns. Any
color can be chosen for each of the two colors in the pattern.
21. GPL'd Source code! Can compile with VC2010, VC2005, or mingw.
22. Online active DRC prevents clearance errors while routing or
dragging traces. Moving traces is free-range and the end points disconnect
no DRC for that.
23. While routing a trace, can push another trace that is in the way while
maintaining clearance on both traces. Only traces/vias/pins/areafills
in the current view are used in the collision detection.
24. Schematics must be hierarchical. Every sheet needs a symbol sheet except
the top level. But the sheets can be interconnected with a bus. Buses
can be a mixed collection of signals. Power connections are global.
It might be possible to make global signals too, but I don't know
how yet.
25. One-to-one correspondence from design layers to gerber layers.
26. Trace length calculation is not valid if there is more than one parallel
path. It's even shorter than the shortest path, so it's not really
useful under that circumstance.
27. Conflicting net trace collisions caused by a component move are deleted.
28. ODB++ export.
29. Help is too sparse. Can't search. Manual is same information. Very
lacking in details and concepts.
30. Can measure freely. No grid snap for measurements, and that's good.
31. Footprint generator can make some regular patterns easily. e.g. BGA
with all the pads having the correct pin numbers.
32. Schematic symbols and component footprints are separate. Assign a
footprint (called geometry by the program) in the schematic by double
clicking the component (no menu choice to do this). A different
geometry can also later be changed in either the schematic editor
or pcb editor and updated in the other with reverse or forward annotate.
33. No reference designator renumbering in the layout editor.
34. No cursor key nudging during move. Movement occurs, but in big steps.
35. No teardrop.
36. Ratnest lines are very helpful during manual routing. It shows the
connection from the route in progress to the nearest destination.
Similar to eagle. No need to toggle between straight-45 and 45-staight
as in eagle though; It does this automatically depending on the cursor
path taken.
37. Mask swell and paste shrink are part of the footprint definition, but
can take on default values at creation time.
38. Produces RS-274X output without using painting. Oops; it creates a
aperture macro for a rotated rectangular pad, but ends up painting it!
Home
Help
Search
Login
Register
