Many technologies for fabrication of microwave circuits are available at Poly-Grames including: printed circuit board on duroid substrates, thin film MHMIC on ceramics, laser machining of metals, ceramics, TMM, etc., and high precision machining on CNC.
IMPORTANT!
Before sending any fabrication file, please take your time and pass the checklist below:
- Does the layout comply with the requirements stated in the document?
- Is the Gerber file exported in the proper format (RS274X, precision 2.4)?
- Does unit is in inch?
- Is the DXF file for drilling in the proper units and format (inches, 2.4, dxf2000)?
- Has the DXF file only one layer, is that layer named as the file?
- Are the holes circles, not segments in the .dxf?
- Did you include the substrate type and thickness?
- If you need a base, did you provide a 2D drawing in DXF? (your drawing software allows you to transform any 3D sketch in a 2D one)
- Did you include all extra information needed to fabricate the circuit and the base?
- Did you rename all your files (Gerber and dxf) correctly?
Please take note, that if your files don’t comply with the requests, we are not able to process them, hence some major delays will occur.
Single Layer PCB
1- Single Layer PCB
Specifications for circuits
- Max size 8’’X 8’’
- Min. line width 5 mils
- Min. gap between lines 5 mils
- Connector spacing 0.5’
- Drawing file: Gerber RS-274X , precision 2.4
- Unit is inch
- Each layer has to contain text with a minimum height of 80 mils and track width 8 mils
- Cutting marks: 200x200x20 mils
- Origin at the lowest left corner of the layout
Single Layer
2- Single Layer with vias
Specifications for circuits
- Plated vias
- Used for large quantity of holes on circuits or if size of hole is critical
- Min. aspect ratio of 2:1
- Center of pad covered in the layout
- .dxf file for holes (precision 2.4)
- Max. circuit size 6’’x6’’
Plated vias or slots
Specifications for circuits
- Same as single layer
- Riveted vias
- Used only if circuit contains less than 15 holes
- Hole 31 mils diameter
- Pad 60 mils diameter
- Center of pad uncovered
Plated Hole
3- Circuits with riveted vias
Specifications for circuits
- Layout files: Gerber RS-274X, precision 2.4
- No drill file required
- Only one hole size: 31 mil
4- Plated Vias
Specifications for circuits
- Layout file: Gerber RS-274x, 2.4
- Hole file dxf, 2.4, single layer
- Holes are filled on the layout file
- Three alignment holes of 66 mils dia with donuts outside of layout
- Aspect ratio for plated hole max 2:1
- Clearance of 10 mils
- Max PCB size 6” X 6”
- Laser cutting area is limited to 7″ X 7″
5- Laser drilling
Specifications for circuits
- For laser drilling use poly-line
- Holes need to be circles, not line segments
- Minimum space 10 mil between 2 holes
- For soft substrates maximum thickness: 60 mils
- For ceramic: 20 mils
- Maximum circuit size 7” X 7”
- Oversize of cutting 2 mils
6- Plated Vias – Gerber and dxf files
Plated vias Gerber file
7- Plated Vias – dxf files
Plated Vias dxf files
8- Clearance
- Spacing of 10 mils min. between hole edge and copper
9- Component assembly
You have to provide the following drawings:
Layout
A component list is required (type of component and quantity)
You have to provide the following drawings:
Component location
A component list is required (type of component and quantity)
10- Component pad spacing
- 0402 Gap 20 mil Pad width 25 mils length 55 mils
- 0603 Gap 30 mil Pad width 35 mils length 75 mils
- 0805 Gap 40 mil Pad width 55 mils length 95 mils
- 1206 Gap 40 mil Pad width 65 mils length 140 mils
- For integrated circuits refer to the datasheet
- Consider that you will have to solder the components manually, leave enough space
11- Assembly box & base
- Drawing of a 2D box
- Flattened (no 3D) dxf file for each side, or SolidWorks file
- Position of hole on drawing should be accurate and at scale
- Unit is inch
- Origin in the lowest-left corner
- Provide all the information needed (thickness, material, etc)
- SolidWorks files accepted
Assembly box
Assembly base
Assembly base
12- Substrate-Integrated-Waveguide (SIW)
- Holes or slots are cut by laser
- Consider an oversize of 2 mils for laser cutting
- Laser cuts only through-hole
- Aspect ratio of minimum 1:2 (minimum hole diameter at least half of substrate thickness) should be maintained for plating
- dxf file precision 2.4, single layer
Substrate-Integrated-Waveguide
13- Partly machined substrate
- The channel is cut by milling, only standard sizes are available. Contact Steve
- Minimum remaining thickness of substrate 10 mils
- Laser cuts only through-hole
- Aspect ratio of minimum 1:2 (minimum hole diameter at least half of substrate thickness) should be maintained for plating
- dxf file precision 2.4, single layer
1- Multi Layer PCB
Specifications for circuits
- In order to make complex RF structures, we developed a method to assemble several substrate layers.
- Epoxy at high temperature and pressure is used to combine the layers.
- The layers can be either printed with via, plated slots or holes
- The final assembly can also be printed, drilled, milled or plated
Top view of a multi layer circuit
2- Side and top view of multilayer circuit
Top view of a multi layer circuit
3- Required files
- Need a 3D drawing to represent the entire circuit
- Plated holes and inner connections are feasible
- If connection is required between two substrates, a plated via is required
- Max size is 2” X 5”
- First substrate is on the bottom
- Text indicating the layer name has to be printed on each layer
- Indicate on the drawing the top or bottom layer
- Ex: S1B ( substrate 1 bottom)
- Gerber file for each layer
- Drill file is a .dxf
- Limited to 7’’ X 7’’ (laser cutting)
- The alignment between substrates is made using 0.125” diameter pins at 2.5” center to center distance
- The layout contains the corresponding donuts of 125 mils internal and 250 mils external diameter
4- Adhesive specification
- Adhesive is epoxy
- ER = 3.5
- Td= 0.03
- Thickness 5 µm
- Solvent resistant
- Hole can be plated through adhesive
Adhesive specification
1- MHMIC Fabrication Process
MHMIC circuit
2- MHMIC without vias
- Circuit has a better resolution
- Max size: 0.950” x 0.950”
- Ceramic Al2O3 10 mil thick
- Min line width: 1 mil
- Min line-to-line gap: 1mil
- Resistor 100 Ω/Square
- Conductor is Au 1 µm
MHMIC without via
3- MHMIC with via
- Max size 0.950” x 0.950”
- Ceramic Al2O3 10 mils thick
- Min line width: 1 mil
- Min line-to-line gap: 1 mil
- Min hole diameter: 3 mils
- Minimum hole covering is 3 mils (ex. hole diameter 10 mils –pad diameter 16 mils)
MHMIC with via
4- Hole Covering
Hole covering
Required files
5- Resistor
- Resistive layer is of 20 nm of Ti under gold
- First step: conductor is etched including Ti
- Second step: resistor is open trough the conductor
Resistor
6- Conductor Gerber file
- The conductor layer is positive mask
- Indicate your name and professor on circuit
- Always print text on layout
- Indicate cutting mark
- Layout: Gerber file
- Need at least 2 test resistors
Conductor
7- Resistor mask
- Negative mask
- Open only the resistor area
- Mask is Gerber file
- The opening is larger than the line by 5 mils
- Alignment is corner to corner of circuit in the cutting mark
Resistor mask
8- Die assembly
- Mounted on substrate
- No power dissipation
- Mounted on base
- Better grounding
- Power dissipation
- For higher frequencies
If you use the S parameter of device manufacturer use the same mounting parameters
Die Assembly
9- Die mounted on substrate
- Die is mounted on alumina with conductive epoxy
- A gap of 2 mils is required between die and line
Die mounted on substrate
10- Die mounted on base
- The step is 1 mil larger than Die
- The cutting hole on ceramic is 2 mil larger than Die
- DXF file for mechanical work
Die mounted on base
11- Wire Bonding parameters
- Wire diameter: 0.7 mil or 18 µm
- Ribbon: 3 mils X 0.5 mil
- For die mounted on substrate bond length is 2 times the die height
- For die mounted on base the bond length is the spacing between pad and line
- Always provide a wire bonding layout
DC connection
- It is impossible to solder a wire to thin film gold
- Small PCB line is added to make interconnection
DC connection
