Drill Hole size drawing when uploading a design

Archive BatchPCB
1

Hi,

I have uploaded my first design in Batch PCB and I am a little bit disappointed. When comes the time to select or re-order the gerber layers, it shows me the drill layer with very big circles at the places of the holes. I do not know if the circles are supposed to be the same size as the holes, if it is the case, there probably is a problem with my file ?

See the screen caption :

http://poildegris.free.fr/Imgbase/batch/funny_drill.jpg

Files are generated with TARGET 3001 in Gerber RS-274-X for the layers and in excellon format for the holes.

Thanks.

2

I have the same problem!!! I spent 2 days creating the design using DesignSpark and all is ok except the drill file. My drill file after uploading looks like larger circles. What is wrong with this file (partial)? Please help.

M48

INCH

FMAT,2

T1C00.025

T2C00.030

T3C00.032

T4C00.035

T5C00.040

T6C00.045

T7C00.088

T8C00.125

%

T001

X00453Y02103

X00453Y02353

X00553Y02053

X00553Y02303

X00653Y02003

X00653Y02253

X00753Y01953

X00753Y02203

X00853Y02103

X00953Y02053

X00953Y02303

X01053Y02353

X01153Y02003

X01153Y02253

X01253Y01953

X01253Y02203

X01453Y02103

X01453Y02353

X01553Y02053

X01553Y02303

X01653Y02003

X01653Y02253

X01753Y01953

X01753Y02203

X01853Y02103

X01953Y02053

X01953Y02303

X02053Y02353

X02153Y02003

X02153Y02253

X02253Y02203

T002

X00253Y02103

X00253Y02203

X00840Y00503

X01578Y00503

T003

X00265Y00865

X00265Y00965

X00353Y00478

X00353Y00678

X00428Y01078

X00428Y01153

X00428Y01228

X00528Y00415

X00528Y00715

X00628Y00415

X00628Y00715

X00653Y01078

X00653Y01153

X00653Y01228

X00665Y00865

X00665Y00965

X00728Y00415

X00728Y00715

X00828Y00415

X00828Y00715

X00828Y00865

X00828Y01165

X00928Y00415

X00928Y00715

X00928Y00865

X00928Y01165

X01028Y00415

X01028Y00715

X01028Y00865

X01028Y01165

3

Further Information:

My file is also Excellon. I do not have an option to create another format. Does BatchPCB support Excellon format drill fiels?

4

Check the Gerbers and drill file with a Gerber viewer, I use GC-Prevue. It’s probably a BatchPCB problem.

5

I did check my file with GC Prevue and it looks fine. I also ran my DRC on my PCB program. I found out what was wrong. I had to add a “,LZ” to the “INCH” designation in my drl file. Without the “LZ” BatchPCB thinks 00.025 is 0.25 so all of the holes are 10 times too big. LZ stands for leading zeroes. Here’s my header:

M48

INCH,LZ

FMAT,2

M72,LZ

Unfortunately my design still generates a “Failed” with no indication of what is wrong.

Henry Arnold

6

Is there a BatchPCB moderator? I think this is a BatchPCB problem. I uploaded my files to another vendor without errors and my board is now being fabricated. I still would like to understand what went wrong.

Henry Arnold

7

Here’s a .drill file I have used successfully on a small PCB. Note the absence of a FMAT,2 line … it assumes legacy simple drilling machine mode (format 1).

M48
INCH
T01C0.0354
%
T01
X+002500Y-001750
X+002500Y-002750
X+002500Y-003750
X+002500Y-004750
X+004000Y-004750
X+004000Y-003750
X+004000Y-002750
X+004000Y-001750
X+005500Y-001750
X+005500Y-002750
X+005500Y-003750
X+005500Y-004750
X+007750Y-004750
X+007750Y-005750
X+007750Y-006750
X+007750Y-007750
X+010750Y-007750
X+010750Y-006750
X+010750Y-005750
X+010750Y-004750
X+010750Y-003750
X+010750Y-002750
X+010750Y-001750
X+007750Y-001750
X+007750Y-002750
X+007750Y-003750
X+001000Y-003750
X+001000Y-004750
X+001000Y-002750
X+001000Y-001750
T00
M30
8

This is an old question but I thought I’d describe a solution I discovered that changed my uploaded drill renderings from big blogs to properly-sized holes:

Open the “Output Plots” dialogue with Shift+P

On any of the design Plots, click the “Output” tab and the “Device Setup” button.

Change the Format values to: “Integer” = 2 and “Decimal” = 4.

Best,

Michael