Frequently Asked Questions
On the following pages, you can find answers to frequently asked questions about printed circuit board technology and related subjects.
In case you do not find the answer to your questions here, please feel free to contact our sales department on telephone +45 7291 2200 or send an e-mail to sales@gpv.dk.
Answers Q1: What are the smallest hole diameter and the smallest pad-size I can use for via holes?
Answers Q1: What are the smallest hole diameter and the smallest pad-size I can use for via holes?
A: The size is determined by the following:
The aspect ratio, i.e. the circuit board thickness divided by the hole diameter, maximum is 8. As an example, the smallest drilled hole that can be used in a circuit board of a thickness of 1.6 mm is: 1.6/8 = 0.2 mm. If the circuit board has a thickness of 2 mm, the smallest drilled hole will be: 2/8 = 0.25 mm.
Minimum pad-size is hole diameter + 0.42 mm on the inner layers, and hole diameter + 0.35 mm on the outer layers.
Minimum drilled hole using mechanical drilling is 0.2 mm.
Other rules apply when using blind/buried laser-drilled vias, please also refer to the HDI section
Q2: What are the smallest conductor width and the smallest spacing between conductors I can use on GPV circuit boards?
Q2: What are the smallest conductor width and the smallest spacing between conductors I can use on GPV circuit boards?
A: Minimum conductor width is 100 micron on an 18-micron base-copper thickness. On a base-copper thickness of 35 micron, the minimum conductor width would be 125 micron. Correspondingly, the conductor spacing is 100 micron and 125 micron; but in case you should be able to accept a conductor spacing of 125 and 150 respectively, this would improve the manufacturability of the circuit board.
Q3: Where do I find information about core thickness, prepregs and dielectric constants in multilayer build-ups with controlled impedance?
A: The Chemitalic Materials section lists all Chemitalic laminate types and prepregs stating also thickness and dielectric constants.
Q4: Where do I find information about advantages and disadvantages of different circuit board surface finishes?
A: The section Surface Finishes section compares the properties of a selected number of surface finishes.
Q5: What data formats are handled by GPV ?
A: GPVcan handle data from all types of CAD systems, CAD postprocessors and Gerber generators that comply with the following standards:
Layer data: Extended Gerber, RS 274 X (Preferred), Gerber, RS 274 D, IPC-D-350 and IPC-D-356
Routing and drilling data: Extended Gerber RS 274 X, Gerber, RS 274 D, Excellon 1 and Excellon 2 and Sieb & Meyer 1000 and 3000
Drawings: Extended Gerber RS 274 X, Gerber, RS 274 D, HPGL, Autodesk DXF and Adobe PDF
Data compression: .ZIP PKUNZIP (Preferred), .LZH LHA, .ARC PKXARC, .ARJ ARJ, .z Unix compress, .gz Gunzip (Gnu unzip) and .tager Unix Archiving. EXE Self-extracting files to be avoided due to risk of virus infection.
Q6: Is GPV able to supply multilayer circuit boards using laminate types other than standard FR4?
A: Yes, please refer to the Materials section
Q7: Dielectric constant and loss tangent are stated by 1 MHz; what are the values by 1 GHz?
A: Regarding GPVs standard FR4 laminates and prepregs (Polyclad PCL-FR-226), the following typical values are stated:
|
Laminate thickness < 0.31” (0.78 mm) |
1 MHz |
100 MHz |
1 GHz |
|
Dielectric Constant |
4.6 |
4.5 |
4.3 |
|
Loss tangent |
0.015 |
0.015 |
0.015 |
|
Laminate thickness ³ 0.31” (0.78 mm) |
1 MHz |
100 MHz |
1 GHz |
|
Dielectric Constant |
4.8 |
4.6 |
4.5 |
|
Loss tangent |
0.015 |
0.015 |
0.015 |
Q8: Can I specify both galvanic nickel/gold and electroless nickel/gold on the same circuit board?
A: Yes, but note that galvanic nickel/gold is plated after electroless nickel/gold. This means that auxiliary conductors must be used to establish electrical connection from the galvanic nickel/gold pattern parts to the production panel border material. The auxiliary conductors will be cut in the routing operation.
Q9: Can I specify both galvanic nickel/gold and HASL on the same circuit board?
A: Yes, and there are two options:
The first option is to use auxiliary conductors to establish electrical connection from the galvanic nickel/gold pattern part to the production panel border material; a typical method is to make connection to the edge connectors. The auxiliary conductors will be cut in the routing operation.
The second option is a so-called selective galvanic nickel/gold, which is a process that is carried out prior to the processing of the outer layers' pattern parts; here there is no need for the above auxiliary conductors.
Q10: What does a standard build-up of an eight-layer circuit board, thickness 1.0 mm, look like?
A: The build-up is as follows:
Cu Foil 18 micron
2 X Prepreg 1080
Lamianate 0.1 mm 18/18 micron Cu foil
2 X Prepreg 1080
Lamianate 0.1 mm 18/18 micron Cu foil
2 X Prepreg 1080
Lamianate 0.1 mm 18/18 micron Cu foil
2 X Prepreg 1080
Cu Foil 18 micron
Nominal thickness is 1.00 mm; calculated thickness is 0.964 mm
Q11: What is the smallest distance between an inner layer pad and the surrounding copper plane?
A: Minimum distance is 0.15 mm in all directions; see FIG 1 below:
