Checked Aperture 10 (0.0050): Failed. Pad Rotation????

Archive BatchPCB
1

Hi All,

I have tried to upload a design to the PCBbatch Bot, but I always get the following error.

Checked Aperture 10 (0.0050): Failed

Error - Aperture too thin

Now, after many uploads I have proved that it is due to pad that was rotated when I created a SMT package library file.

I have also created a PCB with one square pad that I rotated by 45 degrees, which then gives the same error.

The device is a SMT inductor (CLS5D14 by Sumida) The four 8) 8) pads for this device are 1.9mm x 1.6mm which I then rotated by 45 degrees.

Please see http://www.sumida.com/en/products/Produ … No=CLS5D14

I am using PROTEUS ARES PCB package by labcenter.co.uk.

How can I overcome this problem?

I really want to use PCBbatch for all of our boards but can’t seem to get over this first problem.

Any ideas?

Thanks for you help.

Kind regards

Paul Boorman

2

It seems there’s a solution to that problem in this thread.

viewtopic.php?t=9788

I don’t use Eagle, so I don’t know if it will work or not.

-Dave

3

Hi,

Thanks for your reply.

However, this has not solved the problem.

I have edited the pads to give round corners in the hope this may help and I also changed to a solid fill in the pad properties but this has not helped.

I can’t find anything else to change. It just seems like once a pad is rotated it causes this problem.

I really would like to use BatchPCB for our boards so getting over this issue is really important and time critical.

Hopefully, further designs will not use rotated footprints.

If I use the same footprint/package but do not rotate it then I do NOT get this error and the upload/DRC bot check is ok.

Someone out there must have a solution to this problem.Apart from changing PCB packages I not sure what else to try.

I have looked at the rotated pad in Viewmate, and zoomed right in but cannot see any obvious problems.

Any more ideas?

Thanks for taking the time to read this post.

Kind Reagrds

Paul Boorman

4

Could you not make the pads rectangles (or square) and rotate the inductor 45 degrees instead?

5

Some specifics to your problem might help a little more. Overall yes this is in a way a problem with the batchpcb drc bot but considering the user error problems they have had in the past I can respect the bot’s sensitivity. Its also an interesting problem with 2 different cad programs freaking out when a part is rotated.

Anyway, you said you rounded the pads but how much? I found in Eagle that nothing less than 50% on a QFN32 package would work. The part and program you use may require a different amount so as to ensure the pads for the rotated part are drawn with 8mil lines and not 5mil lines which is your problem. Just zooming in to the design wont show you if there are offending small apertures layered to make up the rotated pad as my design did.

In viewmate it is possible to investigate the ‘D Code Table’ which will tell you the various apertures used in your cam file. On the top menu bar towards the right it you will find “Only” with a checkbox, small button (mine has the letter D in it), text window showing an aperture, [<] button with arrow. Click on the button with the left facing arrow to find a menu that shows all the apertures in your design. In there you should find the .005 aperture. Click on the offending aperture and click ok. Then make sure to click the Only checkbox. Now whenever you left click on the design it will only select an aperture of the size you selected. Hunt around on the design until you find all the offenders. Now you will know where the error is occurring and hopefully will be able to find a workaround to solve the error.

Once you see where the error is happening you can go back in to the design and try making some changes to the part library. Try increasing the roundness for example and look at the new cam file in viewmate to see what if anything has changed.

I spent a good many hours troubleshooting my recent design and it really sucks. But keep at it and Im sure youll find a solution. In some ways be thankful that the batchpcb bot bulks at these problems as it would suck to have the board get screwed up on the production line because of too many small apertures.

Best,

B

6

I have just encountered the same problem with Ares outputting Gerber files to the BatchPCB bot.

Apparently when you use a non-standard pad (ie you take a normal pad and rotate it 45 deg) or you use the Power Plane feature to make polygonal pads (my problem) the Ares to Gerber process “draws” the shape using “strokes”.

These strokes are like many many overlapping .0025 traces placed .002 apart. Each polygonal shape is set up as an addition to the netlist in the Gerber file as a “style”, and given a number that starts with D. This D number corresponds to the “Aperture” error number from the BatchPCB Bot. You can only see the D style number when you open the Gerber files in Gerberview and then run the mouse over the traces until you find the one giving you the errors.

Once you examine your Gerber files, you will see that your pad, and in my case my power plane, is made up of a boundary trace, that creates the outline pf the polygon shape, then it fills the shape with many, many parallel traces, that are either horizontal or parallel. When you open Gerber output layer in ARES, you can select each trace that makes up your rotated pad and delete every 3 strokes and change every 4th “stroke” to .010 trace, or every 2 strokes and the third stroke an .008 trace. To do with with my power planes is going to take hours of work. I’m not sure its worth it. It should take you a few minutes for each pad.

Then you re-output the file as a Gerber file, use an external zipper, like WinZip to put the files back together, then you can re-submit zipped files to the BatchPCB bot. You may be able to output all the necessary Gerber Files. At the bottom of the output window, select the option to open the files in GERBERVIEW. If you do this, it might be possible to edit the Gerber Files directly, then re-output as Gerber files to a ZIP. Try it both ways, and post here what works.

This contradicts what ARES says about the Gerber driver “stroke files”, in which is says that the strokes or traces that make up the strokes are the same size as the boundary you select, so that no design rules are violated. I can find anyway or any where to set the size of the traces used as strokes in the polygonal file.

I don’t think you can select a boundary on your rotated pad. I haven’t tried that yet. If you can, be sure the boundary is T8

I have made circuit boards with Gerber files the exact same way at another outfit, but it was more expensive. Apparently they could do .0025 Aperatures without this problem.

:idea: If anyone has any ideas on how to adjust how the Ares Driver sets the stroke value OR knows of a program where I can export the Gerber files to and convert the boundary or the stroke files into a solid pad.

I would greatly appreciate any help.

Thanks.

7

Wow, what luck. I found how to get Ares to perform the proper files.

Maybe there’s a better way to do it, but, this works.

When you output to Gerber, select Open in GERBERVIEW in the lower left hand check box.

When Gerberview opens, these are the Gerber files opened in Ares again.

On the left side of the screen, click the fat yellow T or ZONE MODE

In the column on the just to the right of the fat T, still on the left side of the screen, you will see TRACES at the top and all traces are listed below.

You will note that the “stroke filled” polygon styles D## are listed as TRACES, these are called Aperatures by the Bot, but the ## of the error listed by the Bot is the same. In my case, the power planes were D15 or D16.

Click each one in the TRACES window, then click the E (edit) button at the top of the box, just to the left of the window title: TRACES

A very small new window will open: EDIT TRACE STYLE

Under NAME box, which say D##, is the WIDTH box - this number should not be less than “8th”, if it is less, change it to 8th. Under CHANGES, check the radio button Update Defaults

Click Ok.

Check each of the D## styles new to the Gerber. I found two listed as 2.5th and one as 7th.

Changing these number, then updating defaults seems to change ever .0025 trace into a .008 trace. There are still thousands of overlaping traces, but, it checks out with the bot .

Now, what I did was to save this new Ares file as (FILENAME)_BPCB then I re-generated Gerber files and submitted these to the BOT and the order is placed! It remains to be seen if I actually get it.

It took hours to figure out, but when I started resizing the traces, I did one by mistake and hit the UNDO button, and the computer crashed. The DRC was running on every single one of the .0025 traces. Luckily my board is only 1" x 1.5 inches!

What else was I going to do? Watch American Idol?

Good luck