Problem with Altium Designer

fab drawing altium

AD loads a number of servers into memory. When you shut it down, those servers don't all immediately unload - it's a way of speeding up a restart of AD. If you don't restart AD, they will eventually unload and free memory.

Problem with @ltium Designer

Our assembly contracter are asking for Stencil!
How I can force AD to generate Stencil for SMD components?
Do I need to generate seperate mask for glue dots? If so, how?

Problem with @ltium Designer

One PCB designer was talking about P-CAD 2006, and claim that my needed highspeed feature are avaliable at P-CAD. Are you familiar with P-CAD 2006? I am wonderin is it included in AD6.8 or it is seperate tool?

Because the location, size, and method of applying glue dots can vary according to your company's manufacturing requirements, you have to include the glue dots as part of your component footprints. Normally, you define the glue dot on one of the mechanical (non-signal) layers. When you generate your Gerbers, you include the glue dot layer. No EDA software automatically defines or generates glue dots.

A stencil is produced from a Gerber file, just like any other PCB manufacturing step. Stencils are etched from thin stainless steel, and are used as masks for applying solder paste or sometimes glue dots. Your assembly house is probably asking for the paste mask stencil - you will have to have it made by a PCB fab using the paste mask layer from AD. Be aware that solder paste is controlled by the thickness of the mask and the size of the mask openings. You control the size of the openings with a design rule in AD before the Gerbers are generated - you would define the thickness of the mask in your instructions to the fab.

PCAD is a discontinued product of Altium. Altium Designer replaced it in the product line. It is NOT included with AD6.8.

Problem with @ltium Designer

- Are glue dots implemented in AD libraries?
- I have provided the FAB all layer data, so they are able to make stencil without any furthre data!(?)
- So it does not worth to take P-CAD and try it?

-Glue dots are not implemented in AD libraries, you have to do it yourself
-As House_Cat said, the stencil is made from the solder paste gerber file, so all the fab house needs to create a stencil is that layer.
-I'm not familiar with P-CAD, but I would assume AD shouldbe able to do almost everything P-CAD can.

Problem with @ltium Designer

- What does venting mean in Camtastic tool?(tools->venting)

- What feature or problem the copper area carry? Actually I want to know why we need to calculate copper area?(tools->calc. copper area)

- Is FR4 usable at Microwave freq.? Is it possible to have a composite stack-up for mixed (analog-digital) applications

A venting pattern is an arrangement of dots or stripes placed on inner layers PCB panels so the gases and resin will properly flow outward when the board is heated and pressed in the lamination process. The venting pattern is placed outside the area defined by the board outline. The PCB layout designer does not normally worry about panel venting. The PCB fab adds the venting when they do the CAM setup of a panel of boards.

The calculation of copper area can serve several purposes. It can help with cost estimation for some boards. It can be used to try and balance the amount of copper from layer to layer to prevent board warping and twisting. Finally, it can be used by the board fab during CAM setup to determine how much copper to add in "thieving" areas on a layer to ensure even etching. Modern fab techniques don't generally worry about adding thieving areas anymore. Processes have improved so much that uneven etching due to copper imbalance seldom happens.

FR4 certainly can be used at microwave frequencies, depending on how much loss your circuit can tolerate. I've used FR4 up to 9ghz, and some manufacturers have gone higher than that. Keep in mind that FR4 is not one kind of printed circuit matierial. FR4 stands for Fire Retardant class 4 , and there are many glass-epoxy types and glass-epoxy ratios that fall in the FR4 category. Some of them have impressive dielectric constants and loss factors.

Yes, you can mix a stackup. There are many high frequency materials that are compatible with FR4 lamination processes. I have used Rogers 4350 and 4003 for outside layers, and high-TG FR4 for inner layers on microwave boards. I have also use Taconic TLG materials in a mixed stackup

Problem with @ltium Designer

- I suggest that microwave board design rules and issues are far from the ordinary or even highspeed digital design! Stubs, angles, ... noise, ... become critical isdsues. Which tool do you use for 9GHz PCB design and simulation?

- Is AD able to support blind and burried via?

- Is back drilling fab house related issue or it is related to design tool setup(specially in AD)?

I use a 3D field solver for analysis/simulation. I do my PCB layout in AD. It isn't the software that does good RF design, it's the designer.

Yes, AD does blind and buried vias.

Back drilling is a fab issue, not an EDA issue. You supply the fab with a drawing and instructions regarding what you want back drilled.

Problem with @ltium Designer

- Why we need to care about component height in placement? What problem may arise?

- In IC fabrication the antenna effect is very important; the conductive line may absorb charge particle in plasma etching or other steps, rise the potential and destroy the devices connected to that line in the same manner as EDS do. I am wondering in PCB design and FAB why we need to check it? I suppose that PCB FAB are all chemical process?!

- What does the acid trap mean?

Component height is an assembly issue. You want to be sure that your PCB will fit in the enclosure properly, connector bodies will clear other components, daughter cards will fit in their slots without hitting other components, etc.

The antenna check that is done by CAM software is different from the antenna effect you are talking about in chip design. The antenna check in CAM software looks for tracks that are only connected on one end - you might call them "stubs".

With older etching equipment, fabs worried about pockets created by copper junctions that formed acute angles on the surface of a PCB layer. The acid would swirl around in the pocket during etching instead of flowing smoothly, and cause over-etching of the copper in that area. The acid trap check in CAM software generally looks for angles less than 45deg and reports them. Modern etching equipment uses methods of acid aggitation that pretty much eliminate concern for acid traps. Most modern fabs don't worry about it anymore.

Problem with @ltium Designer

- Sorry now I remmebr the name! he(assembly man) named the problem as shadow problem? It looks to be other issue than "fit in the enclosure properly"

- After running ERC and DRC properly, all stubs must be removed! However, suppose that we still have stub in our design, why FAB is concerned about it? What is the problem? How they fix it?

Your assembler might be talking about component height for the Pick-and-Place handler. Some modern assembly machines use a vision system that measures reflections, shadows, and contrast to allow the machine to "see" the PCB and its components. As one example, Juki makes such a machine ( **broken link removed** ).

He might also be talking about "IR shadowing" where taller components cause non-uniform heating by blocking infrared heating sources used for reflow soldering. That problem is generally solved by using forced convection heating instead of direct IR.

The fab is only concerned about stubs because the CAM software does a check for them. They are acting as a backup for you when they check the Gerber files before they produce the photomasks used for PCB etching. The presence of a stub isn't a problem for fabrication - they just make you aware of it so you can fix it if you want. Over the years, I've had PCB fabricators catch shorts, opens, stubs, drill size problems, etc. They can be your best friend when it comes to checking for mistakes you may have missed. That's why it's a good idea to establish a good working relationship with a fab you can trust - they work as part of your team.