Seetrax Ranger2 XL Gerber import Problems

[Jack Madden]

Hi All,

I am currently trying to import a gerber file that I have generated in Seetrax Ranger2 XL.

I seem to be having a number of problems,

Firstly, the copper track does not show in the PCB Manufacture Wizard; But the tool path is still generated and the tracks are machined correctly.

Secondly, I cannot get the software to recognize a drill file and and I am presented with the error 'The drill file does not match the Gerber file' even though it was generated alongside at the same time. Auto Drill doesn't work and I'm guessing this is because the software can't 'see' the pads (or tracks).

And lastly; although this is not really a problem. Is there a way to edit the PCB in the software? I'm not looking for anything advanced, just the ability to re-position, copy and mirror the tracks etc...?

Thanks.

[Denford Admin]

Is there a way to edit the PCB in the software?

If you want to do that you can try QuickCAM 2D - you normally get one license with a Denford machine.
Gerbers can be imported into QuickCAM and you can then mirror, move, duplicate etc.
However, generating the offset toolpath in QuickCAM will not be as reliable as the import wizard in VR Milling. Especially on complex boards.

Firstly, the copper track does not show in the PCB Manufacture Wizard; But the tool path is still generated and the tracks are machined correctly.

Secondly, I cannot get the software to recognize a drill file and and I am presented with the error 'The drill file does not match the Gerber file' even though it was generated alongside at the same time. Auto Drill doesn't work and I'm guessing this is because the software can't 'see' the pads (or tracks).

Zip up the gerber and drill files and attach them here for testing.

[Jack Madden]

Thanks for the quick reply,

The gerber file has a .ger file extension but a simple rename to .gb0 allows it to be read by VR Milling.
The Drill file is output from Ranger2 XL as a .txt file. Renaming to a .drl allow VR Milling to see it, but upon opening gives me the error I mentioned earlier.

Manipulation of the PCB isn't so much of an issue, I can do all of that in Ranger2 XL. It was more of a convenience thing, not having to edit the original PCB files.

Just FYI I am using a Router 2600 PRO and VR Milling 5.41.0.546. I believe this is not the latest version of the software but I am using a corporate PC with a very strict software approval and automated delivery service. Regular updates are almost out of the question.

Thanks

[Steve]

I have just had a quick look at the Gerber file and can see it does not come into either VR Milling or QuickCAM 2D correctly.

Having tried the AutoSize there seems to be no board size info being exported. The track data is as you say present as the cutter paths are being plotted.

I have used the free gerber viewer online and that shows the circuit OK.

https://circuitpeople.com/

The problem you have with rotate and mirror are carried out on the page of the wizard where you say if it is solder or component side and you also have a flip option. If you could see the artwork this would make sense.

ADMIN will have a look at the file but you may want to check the Ranger software to see if there are any other output settings that would help. Try changing the settings and exporting again.

[Jack Madden]

Thanks for the advice,

I have been through almost every setting in Ranger, some of which gave errors (to do with the dcode table if I remember correctly) and others that made the file completely unreadable.

The Drill file I forgot to mention was exported as excellon; with a .txt file extension. Does this sound right?

I will have a look and see how the board profile is designed and exported if possible. I didn't design the circuit and hardly ever touch Ranger so I'm not very adept with it.

Does anyone know where I can get some info on gerber files so I can have a read and hopefully spot a problem?

Thanks

[Denford Admin]

Not sure yet why the paths are being created but the tracks aren't shown but that will take longer to figure out
I can see that the hole pads are filled - they need to be open in the middle for autodrill to know where it should be drilling.
I think that your drill file will also work once we get the tracks to load in properly - I think it's unhappy because its comparing the drill data to the tracks which it can't see. In fact, if you open any one of our example .gb files and load the drill file in, it reads the positions ok - meaning you can just output the drilling cycle at the end of the wizard.
Try some different settings on your Gerber output while we look at why the tracks aren't being shown properly.

[Denford Admin]

Does anyone know where I can get some info on gerber files so I can have a read and hopefully spot a problem?

This .pdf is the standard we worked to, although not all the commands are supported.
If you spot a difference between a .gb file that works and one that dosn't then let us know and hopefully we'll be able to support it in the next version

Here is the link to get the Gerber format specification:
https://www.ucamco.com/downloads.php

[Steve]

Hi,

I use a package called Easy-PC which has various setup options For drilling I use the NC Drill settings in Excelon format. I attach the settings,

[Steve]

Gerber settings I use are as below.

[Steve]

Note in both the Drill and Gerber setup windows there is a plotting limits setting in this case set to 36"

If this is not set then the tracks do not import,

[Jack Madden]

I will have to have a look at Ranger on Monday when I get back to work. I know there is definitely a setting for unfilled pads which I will try, and also I'm sure I've seen something to do with the plot area.

As much as I'd like to get rid of Ranger and swap it for something like EasyPCB, I don't think that's an option. Again this is due to our "Software Shelf" at Cummins and me not having admin rights to any of the PC's. I'm going to try and generate some Gerbers with Eagle this weekend and bring them into work to try. Hopefully if they work I might be able to spot a difference in the files and find out what's wrong.

Although using the drill file would be preferable, if I can get the auto drill working (even just to spot the holes) then I can manually drill what I need. we have a minature pillar drill in the workshop ideal for the job. We will possibly make around 10 - 15 PCB's a year on the machine as it is mainly used for engraving Aluminium Panels so it's not a huge inconvenience.

I will report back on Monday

Thanks

[Denford Admin]

generate some Gerbers with Eagle this weekend

I've had Eagle working in the past and the last post here shows how to configure it for our import wizard:
viewtopic.php?t=2127

[Denford Admin]

Ok I've found the problem:
It's the very first few moves which draws the outline rectangle of the board. The aperture it uses (D10) is defined as a circle of 0.0000" diameter:
%ADD10C,0.0000*%
This caused the problems drawing the tracks (ie, it was trying to draw a track of zero width)
I'm not sure whether a zero size aperture should be allowed, but the next version of VR Milling 5 and QuickCAM will force the minimum aperture size to be 0.001mm to avoid this in the future.

[Jack Madden]

Fantastic that did it. I can't believe I didn't notice that.

As it turns out we are using a 12 year old version of Ranger2XL, we are just in the process of updating it. I hope that fixes the rest of the issues.

I think I may have discovered a new issue. When using auto-drill the cnc output does not specify a tool change and so just "spots" the holes with the engraving tool; Although this is easily overcome by manually adding code to the editor (Tool change AND Spindle start).


Thanks again for the help.

[Denford Admin]

You may need to turn off Pilot drill only on this screen.
The autodrill looks for different size pad holes and assigns a tool number to each one.
In the .drl file I loaded here, tool 2 and 3 are called with an M06 near the end of the program.