What is Altium Dashboard on new release winter09

[Johnson]

@ltium's Dashboard

Again NB2DSK reference board,
1) Is LCD as a component? Where is the LCD connector? Is it connected to main board by cable? Indeed I am looking for design rule in that area! How we can put one smaller component beneath of taller one without drc violation?
2) There are two special mounting holes for that TFT/LCD with more than 4-way thermal connector which is not definable in design rules? How we can manage it?
3) Around voltage regulator with KTT package, special via/hole array is used which act as a heatsink. Those holes are not part of component, how we can create it and important issue in the case of similar components, how to reuse it?

 

[House_Cat]

Re: Altium's Dashboard

You can download the dashboard from https://www.altium.com/community/downloads/?

1 - The LCD is mounted on the motherboard. It is part HITACHI_TX09D50VM1CAA, and it is flex cable connected to connector LCD1 at about 8449, 1952. You'll see two large arrows on the top overlay pointing toward the connector. The component height design rule relies on the component body to determine clearances. You can give the body a height above the board which allow smaller components to be placed under it. In this case, the applicable rule is "ComponentClearance_Top".
2- The LCD mounting holes are not connected to anything, so I don't know which holes you are talking about.
3- Altium Designer allows you to define a pad as a slot. Those holes are actually sloted pads rotated 45deg. Double click on one of them and you'll see how they are defined. They can be placed one-at-a-time anywhere on the PCB, or they can be included in a footprint. When you generate your NC drill files, you can also automatically generate route paths for the slots. One of the neat things about slotted pads is that they automatically create slotted anti-pads on any planes in your stackup. To create the pattern of slots used on this board, the layout designer probably used what is called "rubber stamp" to place the first row, then copied and pasted the rest from the first row. I would have made a component, but every designer has their own way of working.

 

[Johnson]

@ltium's Dashboard

- The build number of dashboard (15946) is different from main AD distribution (15895)! Does it mean that update is released?

- Is 45 deg. placement acceptable for pick&place job?

- Same as controlling the visibility of components in 3D, can we control the visibility of internal routing layers?

- There are some polygons in the board without solder mask, but not connected to any net(for example at location: 5348mil, 921mil). What is the usage of them? ESD related issue? if so, why there are not connected to GND?

- A strange shape (spark gap) is on back side of board beneath the ESD Touchpad? Do you know what is it?

- regarding the free FDIC on the board (not related to BGA component), usually fab ask about them, is there any rule where to put them, and how many is enough?

 

[House_Cat]

Re: Altium's Dashboard

The development of the Dashboard continued past the release for W09. No, there's no update for W09 this soon.

Yes, you can have 45deg objects for pick and place. You can have any angle - it's up to your assembly house to tell you if they have any limits.

Of course you can control visibility of layers. You can hit "L" in the 2D display mode and turn layers on or off. You can also set up Layer Sets by clicking on the "LS" box in the lower left corner of the PCB Editor screen. You can also right click on the layer tab at the bottom of the screen and turn the layer on or off.

Those fills are just mechanical landing pads for connectors and daughter boards.

It's a spark gap. Look on the top overlay, and you'll see instructions to "Touch Here First". Any static on your body will be discharged to the shield ground. The spark gap also serves to discharge the board ground to shield ground which should be the same as mains ground.

IPC states "Global and/or panel fiducials should ideally be located on a three point grid based system, with the lower left fiducial located at the 0,0 datum point and the other two fiducials located in the positive X and Y directions.

Global fiducials should be located on all PCB layers that contain components to be mounted with automated equipment. This is true even if the circuit design contains no fine pitch (<= .020” pitch) components, as most modern assembly equipment uses vision recognition for PCB alignment."

 

[Johnson]

@ltium's Dashboard

- Regarding sloted pads, does it add some amount to mfg cost or is a normal drilling? I want to know that sloted pads requires CNC operation or not?

- In manufacturing process, when drilling is done? Indeed I want to know how they allign layer masks, which looks to be very important.

 

[House_Cat]

Re: Altium's Dashboard

Slotted pads are routed, not drilled. Whether or not it adds cost is up to your fab. The one I use (Gorilla Circuits) doesn't charge extra.

If there are no blind or buried vias, the plated hole drilling is done as the next step after lamination of the board. The holes are drilled and slots to be plated are routed, cleaned, coated with carbon, plated, and cleaned again. The board is then drilled and/or routed again for the non-plated holes and slots, and the holes are cleaned. If you have any gold, silver, or tin plating it is done next. Then the soldermask is applied, and finally the silkscreen is applied.

Masks are optically aligned with the finished board, as are the silkscreens.

 

[Johnson]

@ltium's Dashboard

I beleive that in AD library element is not related to stack up, and we can change stack up and use the same library, but in Allegro, based on padstack, library is related to specific stack up. So by changing stack up we need to develop new library, is there any method to avoide it?

 

[Johnson]

Re: @ltium's Dashboard

I beleive that in AD library element is not related to stack up, and we can change stack up and use the same library, but in Allegro, based on padstack, library is related to specific stack up. So by changing stack up we need to develop new library, is there any method to avoide it?

-- Any sugesstion?

 

[House_Cat]

Re: Altium's Dashboard

There's really no difference between AD and Allegro footprints when it comes to layer specific objects. You can define a library footprint for just the top and bottom layers, and then use it on a multilayer board. Padstacks are defined in similar fashion in both AD and Allegro. W09 has added via stacks which makes it even more like Allegro.

What makes you think that component footprints are locked to the stackup in Allegro? The same library component can be used in 2 layer, 4 layer, 6 layer, etc.

 

[Johnson]

@ltium's Dashboard

What makes you think that component footprints are locked to the stackup in Allegro?
A. I exported a library from a board and tried to used it in a board with different layer count, but it comes with some error and warnning.

 

[Anonymous_Ricky]

@ltium's Dashboard

The error will be shown only if the naming is not same in libraray and board.
But if the layer naming is same than there wont be any problem as mentioned by HC