Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Rectangular holes - how to solve this problem?

Status
Not open for further replies.
E

Eugen_E

Full Member level 6
Joined
Nov 29, 2004
Messages
383
Helped
44
Reputation
86
Reaction score
11
Trophy points
1,298
Location
Romania
Activity points
2,862
drill symbol

Hello,
This may seem a silly question. Many power connectors have pins as metallic sheets with width of about 2-4mm and thickness of 0.3-1mm, thus the pins are not round.

To ensure correct insertion in the past I used pads with huge holes for the power connector, like 3mm. This looks ugly and also is hard to solder, because the solder tends to flow in the hole, the pin being thin.
Can we specify rectangular holes like 3x1mm? Is this option available in the CAD programs, and how it will translate in the drill files? Are the board manufacturers capable of making those?
 

how to make rectangular holes

hi,
what I do is I provide multiple circular drills of size equal to width of pad drill at the same loaction with little offsets so that they give me the required length of the pad driil the drill.For example I have a pad with drill 0.3x0.6mm what I will do is I will take a pad with drill of 0.3 mm an pad size 2 mm then I will put 0.3 mm drill on teh same pad with an offset of 0.15 mm .
hope it is clear to you .

Regards,

Ricky
 

    E

    Eugen_E

    Points: 2
    Helpful Answer Positive Rating
I provide multiple circular drills of size equal to width of pad drill at the same loaction with little offsets
Click to expand...
You should be aware, that an attempt to drill holes as you specified it very likely would break the drill tool. So the PCB manucturer has to filter it and replace it by a milling contour. You should check, which techniques are available at the manufacturer and prearrange if you should define either a placeholder drill tool or a milling contour in your CAD data.

P.S.: I asked a manufacturer, who is doing most of my prototype PCBs (www.britze.de), and he is usually milling the reactangular throughplated holes, minimal tool size is 28 mils/0.7 mm. A centerline with the respective tool diameter would be preferred in NC data. Cause milling with small tool is rather slow, the highest applicable tool diameter should be used.
 

    E

    Eugen_E

    Points: 2
    Helpful Answer Positive Rating
I am talking of a pad size as shown in image with circular drills and rectangular pad size.
[/img]
 

Yes I understood this. My comment was exactly on your suggestion. It can't be drilled as specified. NC machine data processor is required to remove all overlapping drill holes to avoid tool breakage, in most cases, the CAD postprocessor already does.
 

What you would need to do is specify these holes on the drill drawing so that the board fab house knows whats needed.

They will then route them out with the router/drilling machines before plating.

If you want to be able to show the start & finish you put a single drill at each end, but it MUST be identified as a slot in the drawing.
The fab house then make adjustments to obtain the finished slotted pad.
 

    E

    Eugen_E

    Points: 2
    Helpful Answer Positive Rating
Hi fvM and cyberrat,

Thanks for you comments.
These were really helpful .

Ricky
 

Thanks for the replies. I thought there is standard method.

FvM - placing a center line is the most convenient. A hole should also be placed in center of the pad, or only the line?

cyberrat - this solution is "acceptable", but how to place 2 holes on a pad? I'm using Orcad, and the pad should have a typical geometry with a single hole in center. The holes should be placed after post processing, by editing the files resulted?

Anonymous_Ricky - I don't think it can be done that way because the CAD software will show errors for minimum spacing, etc; the drill bit will break, someone who uses a professional CNC told me it's illegal to place overlaping holes.
 

I do it by making special pads & adding them in the locations required, in addition to the pads for the part.

This is because the CAD software does not cope with slotted pads.

Ideally it would, till then it is best noted in the drawings supplied to the fab house.
 

I have recently had boards made where I changed the component pad hole to a slot. I got them back with a slots and the power plug fits perfectly. I assume that they were routed but did not ask :)
 

The easy way would be for the connector manufacturers, to make only round pins.
 

The most important aspect is to make unequivocal production data and to avoid possible misunderstandings by the PCB manufacturer. In many projects, production data is passed to an assembly house that orders the PCB. If possible at all, the data should be clear without additional explanations. (A text file describing the gerber and NC files is often used, but you shouldn't trust, that it's actually read).

A separate NC file for throughplated, milled holes or slots would be the most clear solution, to my opinion, but other solutions as suggested in the discussion are applicable as well. With most CAD tools, some manual action in postprocess is probably necessary to generate separate files.
 

FvM said:
The most important aspect is to make unequivocal production data and to avoid possible misunderstandings by the PCB manufacturer.
Click to expand...
I've just exparienced this problem. I have a board with a DC jack that throughole "blade" pins. I usualy do the layout and order board fab myself, but this time another guy did it for me. He specified something for the blade connectors. But instead of oval slots 4x1mm the manufacturer made oval pads on top and bottom with two holes at the ends of the pads.
 

cyberrat said:
Then perhaps either his drawing did not specify the holes correctly or the fab did not read the drawing.
Click to expand...

It's probably the latter (the fab did not read the drawing) or the fab (PCBexpress/Sunstone) just doesn't mill slots and decided to ignore this discrepancy instead of reporting it back to us while putting our boards on hold. This was our second rev of the board. The first rev was made by a different fab and the slots were milled correctly.
 

Dear friend Eugen_E,

Your problem is, how to give the Rectanguler hole to fabricators.

When the Pad creation, give a small circular hole(Via size drill size also ok) for that rectangular hole, but make sure your pad is rectangular only.

While creating gerber, take the drill symbol of that rectanguar Pad, and mark in the gerber it self, it is a slot of 4MMX1MM like that.


Then the facricators takes the x y cordinate of that drill symbol and make the solt which is in that same X y co-ordinates.

Make sure, each slot drill symbols should different from other slots and other circular drill symbols.


Best regards
R. Balasubramaniaraju
 

Dear friend Eugen_E,

Find the attached PDF file of slot dimenstions.
 

Dear friend,



In this file bottom connector is a USB connector, in that two rectangular slots are there. Find , how i mention that in the gerfile. See in the drill chart i mentioned the 43.3 as drill dia of that solt and i mentioned in the down side of the gerber with the drill symbol as a slot.

then the fabricators make the slot which x and y cordinate are same to the retangular drill symbol.


Thanks,
R. Balasubramania Raju
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top