temp gerber md

b8d42644 · yuichitamiya · 9eb39343 · b8d42644
Commit b8d42644 authored 2 years ago by yuichitamiya
--- a/docs/Instruction/tips/pcb_gerber.md
+++ b/docs/Instruction/tips/pcb_gerber.md
+# PCB sending out from Eagle to board house
+
+Ref. [Export Gerber file from Eagle_JP](https://www.fusionpcb.jp/blog/?p=596)  
+Ref. [seeed FusionPCB blog 基板製造の仕様_JP](https://www.fusionpcb.jp/blog/?p=1217)
+
+## Board house
+
+Seeed [Fusion PCB](https://www.fusionpcb.jp/)
+
+## Eagle
+
+### Relation Eagle layers and Gerber file
+
+Eagle Layers |Gerber and drill file|<br>|Single side PCB milling
+--|--|--|--
+1 Top<br>17 Pad<br>18 Vias|Top Copper (.GTL)|銅箔パターン（おもて面）|1 Top<br>17 Pad<br>18 Vias
+16 Bottom<br>17 Pads<br>18 Vias|Bottom copper (.GBL)|銅箔パターン（裏面）|-
+21 tPlace<br>25 tNames|Top Silkscreen (.GTO)|シルク印刷（おもて面）|-
+22 bPlace<br>26 bNames|Bottom Silkscreen (.GBO)|シルク印刷（裏面）|-
+29 tStop|Top Soldermask (.GTS)|ソルダレジスト（おもて面）|-
+30 bStop|Bottom Soldermask (.GBS)|ソルダレジスト（裏面）|-
+20 Dimension<br>46 Milling|Mechanical (.GML)|Board Outline<br>基板外形|[![](../images/pcb_gerber/attention.png){width=100}](#board-outline)<br>48 Document
+Vias<br>PTH<br>Holes|Drill Layer (.TXT)|ドリル|[116 centerDrill](http://academany.fabcloud.io/fabacademy/2021/labs/kannai/site/instruction/tips/Eagle_Holes_making_shortcut/)
+
+### Board Outline
+!!! Attention
+    ![](../images/pcb_gerber/attention.png){width=100}  
+    For PCB milling with mods, *48 Document* is used as board outline and 20 Dimension is always larger than board size to make the outline milling path.  
+    But for Gerber file, **20 Dimension** will be board outline.
+    ![](../images/pcb_gerber/board_outline_document.png)  
+
+    Move **Dimension(yellow lines)** to the board size  
+    ![](../images/pcb_gerber/board_outline_dimension.png)
+
+
+## Steps
+
+<hr />
+=== "Step 1: CAM Processor"
+    ![](../images/pcb_gerber/CAM_Processor.png)  
+
+=== "Step 2: Load job file"  
+    System Examples -> Third Party -> Seeed Fusion -> SeeedFusion_2_layer.cam   
+    ![](../images/pcb_gerber/seeedfusion_2_layer.cam.png)
+
+=== "Step 3: Process Job"  
+    ![](../images/pcb_gerber/process_job.png)  
+
+    Saved as .zip file
+    ![](../images/pcb_gerber/gerber_zip.png)  
+
+    !!! Note
+        **No need to unzip**  
+        If unzip the zip file, these are included
+        ![](../images/pcb_gerber/gerber_unzip.png)  
+
+
+
+
+## Panelize and V-cut (面付けとV-cut)
+
+Ref . [V-cut_JP](https://westgate-lab.hatenablog.com/entry/2021/02/07/150840#v-cut)
+
+### Why?
+
+```
+The manufacturing cost per board can be reduced by manufacturing multiple boards as a single board by laying them together.  
+If you specify V-Cut between the boards, you can divide it with your own hands.
+
+面付けして複数の基板をまとめて1枚として製造すれば、基板1枚あたりの製造コストを下げることができます。
+基板間をV-Cut指定しておけば、自分の手でパキパキ分割することができます。  
+```
+
+### Basic rule  
+
+Ref. [Panelize and V-cut_JP](https://www.fusionpcb.jp/blog/?p=1233)
+
+1. Draw V-cut line on 20_Dimension layer in Eagle
+1. Impossible to V-cut on Round board shape. V-cut line should be straight from the edge of board to the other side of the edge
+1. Add mark "V-CUT" on 20_Dimension layer as below
+
+![](../images/pcb_gerber/Vcut_small.png)
+
+4.Distance between V-cut line and Cupper line shoud be more than 0.4mm
+
+## How to do
+
+Ref. [Panelize and V-cut in Eagle_JP](https://westgate-lab.hatenablog.com/entry/2021/02/07/150840#v-cut)
+
+<hr />
+=== "Design board in Eagle"
+    ![](../images/pcb_gerber/sensorboard_sch.png){width=300}
+    ![](../images/pcb_gerber/sensorboard_brd.png){width=300}
+
+=== "Panelize (面つけ)"
+
+    Tool -> Panelize...  -> Execute
+
+    ![](../images/pcb_gerber/panelize.png){width=400}
+    ![](../images/pcb_gerber/panelize_execute.png){width=170}
+
+    !!! Note
+        Layers will be Copied     
+        - 25 tNames -> 125_tNames  
+        - 26 bNames -> 126_bNames  
+
+        ![](../images/pcb_gerber/layer_before_panelize.png){width=200}
+        ![](../images/pcb_gerber/layer_after_panelize.png){width=200}  
+        ![](../images/pcb_gerber/sensorboard_brd.png){width=400}
+        ![](../images/pcb_gerber/sensorboard_after_panelized.png){width=400}
+
+=== "Copy all layers"
+
+    Show all laysers  
+
+    ![](../images/pcb_gerber/layers_select_all.png){width=400}
+    ![](../images/pcb_gerber/layers_show.png){width=400}
+
+    ![](../images/pcb_gerber/important.png){width=100}  
+
+    - **Move mouse pointer to (0,0)**  
+    - Ctrl + A
+    - Ctrl + C
+    - Ctrl + W -> Save -> No
+
+    ![](../images/pcb_gerber/0,0_ctr+a_ctr+c.png)
+
+=== "Paste in new board in Eagle"
+    Open new board  
+    ![](../images/pcb_gerber/new_board.png){width=400}  
+
+    Set grid as same as the original board  
+    ![](../images/pcb_gerber/new_board_same_grid.png){width=400}  
+
+    Paste (Ctrl + V ) at (0,0)  
+    ![](../images/pcb_gerber/panelized_board_past1.png){width=400}  
+
+    Paste (Ctrl + V ) just next to the previous one  
+    Two **J1**s exist in one board, not continuous numbers  
+    ![](../images/pcb_gerber/panelized_board_past2.png){width=400}  
+
+    Paste (Ctrl + V ) until 100 x 100 mm size as minimize the cost     
+    ![](../images/pcb_gerber/panelized_board_past100x100.png){width=400}  
+
+    Redraw all Dimension line with Line Width 0  
+    ![](../images/pcb_gerber/dimension_redraw_line_width0.png){width=400}  
+
+    Add Text **V-CUT** on the same layer (20 Dimension)  
+    ![](../images/pcb_gerber/dimension_V-CUT_TEXT.png){width=400}  
+
+=== "Choose copied Silk layers in Gerber"
+
+    !!! Note
+        To make Gerber file, select 125_tNames, instead of 25 tName  
+
+        - 25 tName continuous numbers
+        - 125_tName un-continuous numbers
+
+        ![](../images/pcb_gerber/gerber_layer_25_tName.png){width=300}
+        ![](../images/pcb_gerber/gerber_layer_125_tName.png){width=300}
+
+    ![](../images/pcb_gerber/top_silk_25_tName.png){width=300}
+    ![](../images/pcb_gerber/top_silk_125_tName.png){width=300}  
+
+## Cost
+
+- 25 x25mm x75P:  18.32USD -> 18.32/75= 0.24USD/board
+- 100x100mm x10P: 4.9USD -> 4.9/(4x4 x10)= 0.003USD/board
+
+![](../images/pcb_gerber/cost_25x25x75p.png){width=250}
+![](../images/pcb_gerber/cost_100x100x10p.png){width=250}  
+
+## Round board shape
+
+!!! Attention
+    V-CUT is only accepted when the board shape is made by straight lines. But in case to make round corner shape, this is how to do it.
+
+Ref. [Round board shape_JP](https://westgate-lab.hatenablog.com/entry/2021/02/07/150840)
+
+![](../images/pcb_gerber/kadomaru.jpeg){width=300}
+
+```
+It is OK if you select a line with rounded corners in 20_Dimension and draw the outline of the board. Width is 0.
+
+20_DimensionにLineで角丸のラインを選択して基板外形を描けばOKです。Widthは0です。
+
+```