| T O P I C R E V I E W |
| tswelectronics |
Posted - 23 Dec 2013 : 13:48:16
I used the intelligent gerber import feature years ago and did not have much success with it. Has there been many improvements over the years?
I have a TI reference design I want to import to work on and need the drill holes as well. Has this now been supported?
Thanks
Trev |
| 9 L A T E S T R E P L I E S (Newest First) |
| Peter Johnson |
Posted - 09 Nov 2018 : 12:11:51
There's a different issue here, not directly related to the importer. that is, with a viewer, all it has to do is show an image, plus, perhaps, the underlying structure of the commands which created the image.
With Easy-PC, it's very different, as the information has to be translated into structures supported by Easy-PC. By and large, negative structures aren't supported, so even if the command is read, there's nothing the program can do with it. That's generally true of any Gerber macros (or macro type commands). They have to be ignored because the program has nowhere to put the information.
Changing this in any meaningful way would require a disproportionate amount of development resources to achieve a meaningful result, so it's not going to be a high priority task! |
| edrees |
Posted - 15 Aug 2018 : 11:41:31
I've just stumbled across another failure in both "standard" and "Intelligent" Gerber importers. Both fail with %LPC*% gerber command (but does give a message,- "Warning (line nnn): File contains 'Clear' or 'Negative' shapes which are ignored"). The result is that a poured area now floods over signal tracks shorting the whole lot out.
Peter's suggestion above quote:
The trick here is, if you know there's a problem, import the affected layer(s) using the basic importer, delete the fill, leaving the boundary, then recreate the Gerber files minus fill
does help, but I think this leaves a lot to be desired from a additional cost optional package.
Even "freebie" Gerber importers (including Kicad) seem to handle this command with no issue, so I'm rather surprised to hear No.1's policy to "only handle elements plotted in the normal LPD state. " Perhaps No.1 should tell Ucamco to stop using the %LPC*% gerber command!
|
| Peter Johnson |
Posted - 05 Mar 2014 : 11:25:35
The basic Gerber importer has always been just that. a basic Gerber importer. That means that it can't handle drill information as this isn't Gerber - it's Excellon.
Obviously this is less than satisfactory, but there are requests for this to be changed on the system.
What catches more users out with the intelligent Gerber importer is the settings for the Excellon file (or files). Unlike Gerber, Excellon files do not contain format information, so the scale has to be set correctly when importing them. If you've got the relevant information from when they were produced, it's relatively trivial to set the import correctly, otherwise it's a case of checking in a Gerber viewer to find which ones make the drill data line up with the pads. If the scale is incorrect, holes that don't match a pad, i.e. most of them, are simply ignored, and it looks as though the import has failed.
The issue with importing planes into the intelligent importer is that the planes are built up out of a huge number of lines. The program has to match every single line to attempt to correlate nets. This process follows a square law, so it's relatively easy to generate ridiculous run times.
The trick here is, if you know there's a problem, import the affected layer(s) using the basic importer, delete the fill, leaving the boundary, then recreate the Gerber files minus fill.
These will import relatively quickly (but be aware that the alignment may need correction), and the 'Change Shape Type' function can be used to convert the residual profiles into pour areas. |
| edrees |
Posted - 13 Jan 2014 : 17:23:17
Markpsu,
Check your "FLASH" settings on the Input dialogue. Vias/pads normally import OK apart from the fact that you will loose "pad-shape" information. Drill holes with no electrical parameter may not import properly.
Unfortunately, the "Intelligent" Gerber Import feature hasn't received much (any?) attention for many years and has always been disappointing. |
| markpsu |
Posted - 13 Jan 2014 : 16:30:50
I have XP and have just recently used the intelligent gerber import. None of the drill holes or vias made it through. I find the importer better than working from scratch, but it requires a lot of re-work. We have a real need to import gerbers created by an HFSS simulator. I hope they make some improvements in this area. |
| tswelectronics |
Posted - 24 Dec 2013 : 11:43:21
Thanks for the information, Iain.
The reference design I want to import is an RF based board so I wanted to import the exact tracking to ensure the radio works or at least give it the best chance of working.
Does it import drill holes properly with XP as well?
Trev
|
| Iain Wilkie |
Posted - 24 Dec 2013 : 07:53:02
On the contrary, although not perfect I have used it on numerous occasions in the past for doing various jobs. However that was on earlier versions of EasyPC and I have always used XP Professional.
I have just upgraded to Windows 7 Professional and running EasyPC V17 and I tried it on a wee job the other day and it gave absolute rubbish output !
Could read the files in GCPrevue but the Inteligent import was completely useless. So wether its due to V17 or WIN7, I don't know !
Iain
|
| tswelectronics |
Posted - 23 Dec 2013 : 14:17:34
Thanks for the reply. All I have to say really to Number One is...Tut! |
| edrees |
Posted - 23 Dec 2013 : 14:04:33
Hi Trev,
I recently tried to import a design recently which had large flood planes on all layers. This resulted in enormous file sizes that then became unworkable/unstable.
Despite my moans over the years, "Intelligent" gerber import seems to have received little if not no improvement over the years. I'm still very disappointed with it.
Pad shapes still remain circular as far as I can see.
I don't trust it unless it's a very simple job.
|
|
|
