Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
Actually I do not know what rule I must consider based on the soldering method? And for SMD components, during soldering what happens for the components which are on the other side? how assembly line prevent them from desoldering and falling down?
On a board with components on two sides, the assembler would apply glue dots to hold the components in place before applying the solder paste. The glue holds the components while reflowing the opposite side. The glue mask is an additional Gerber file that would be produced. Glue masks are used in both reflow and wave soldering.
There are several considerations for each type of soldering. For example, with reflow soldering, care should be taken to keep the solder pads approximately equal in area. This prevents "tombstoning" - a condition where the surface tension of the solder pulls the component into a vertical position. For manual soldering, you need to provide a bit of extra room on component pads for the soldering iron contact. For wave soldering, component orientation and spacing is important to avoid skipping or starving a nearby joint of solder.
There are several books that can provide information about manufacturing processes. One of them is "Surface Mount Technology: Principles and Practice" by Ray P. Prasad. Another is "Printed Circuits Handbook" by Coombs.
Some high power components use the PAD on bottom side of pakage as heat sink, and it is recommended to solder this pad. Examples are TPS54610, TLK2501, ... and also components with KTT pakage from TI, TO263-5, ...
Glueing these component may prevent thermal PAD soldering and is not acceptable. Is it a rule to do not put these components on back side?
(But I remember that I saw boards with this type of components on back side!!!)
My PCB fab puts a series of string on board area, and use this codes in order to archive the films. I am wodering do the fab has the right to do that and is it part of fab rules? or I can force them to put this code out of board area?
The glue that is used is not a big blob of glue, but rather just small dots. It does not interfere with soldering.
The fab should never put anything on the board unless you authorize it. I usually tell the fab not to put their logo on the board. If you want their date, QC marks, or production codes placed in a specific way, just tell them. They are in business to make a board for you - not for themselves. There's no rule that says they have to put marks on your board. They do it for their own convenience to identify the board in case of future problems or production. Most fabs make extra boards when you order. The code helps them identify the board if you return a defective one for replacement. It also helps them identify the project in the future if you order more of the same board - they don't have to repeat all of the internal CAM work if they can refer to what they originally did.
after receiveing board, how we can be sure that fab has done the e-test compeletly and successfuly? is there any specific report that we can ask them about it? indeed I need to be sure that board electrically iis ok before starting the assembly process.
A new book appreard in the forum dealing with PCB design on OrCAD, I found it useful. with full of fig and examples. It may worht to recommend it to other pcb starter . I am looking for the same for allegro!
Can I exepect the SODIMM connector to be available in AD?
You don't usually get a detailed report from the fab. The will simply report pass or fail for their QC checks. If a flying probe test is done, it too will just be a pass or fail. The flying probe checks the board against either an IPC-D-356 netlist you have provided to them, or a netlist they have generated from the Gerber files.
The responsibility to ensure that the board is correct before stuffing it remains with the designer. The fab can only check that the board matches the files you provided to them.
You should learn not to rely on footprints from any EDA libraries. There is no such thing as a "standard" footprint that works for all manufacturers. There are many variations on every footprint - mounting hole sizes and positions vary, thicknesses vary, etc. The AD library editor makes it easy to lay out your own using the datasheet for the specific brand of socket you plan to use. SODIMM sockets come in one or two slot thicknesses and three different pin counts (72, 144, 200), and are made by at least a dozen manufacturers. Not even the libraries that you have to buy separately, such as PCBLibraries, come with SODIMM footprints.
1. Some EDA packages have a special dedicated layer for glue dots. In Altium Designer, you would use a mechanical layer when designing the component footprints in the library editor to define the glue dot. That mechanical layer would then become your Gerber Glue Dot Mask.
2. DXP was released about 4 years ago. Since then, the IPC has released a new standard for PCB footprints (IPC-7351A). The footprints included with the newer Altium Designer have been updated to the new standard.
3. The cost of gold plating depends completely on the fab you are using. You'll have to call them and discuss their prices. It would probably be based on the square inches of copper on your board, the number of boards you are ordering, and the turnaround time you specify for board delivery.
4. Any good CAM editor can reconstruct a netlist from the Gerber files and the drill file. It is done by the software analyzing the connecting copper and the location of the plated holes. It's usually just a menu selection in the software. The software does all the work. If you look at CAMTASTIC in Altium Designer, the command to extract a netlist is in the menu at "Tools--Netlist--Extract". In CAM350, it's "Utilities--Netlist Extract".
The AD new update to 6.8 is released, it containe more than 250 fix to bugs in all! Also new features are added, what is your opinion about this new features?
WE CAN MAKE FILM FROM OUR PCBs BY 3D
Demo Videos are avaliable at Altium,
Added after 1 hours 28 minutes:
Is it possible to import netlist to AD? I want to do schematic and generate netlist in OrCAD and import it to AD and do PCB design in AD! It may fix the original problem.
No, you can't import an Orcad netlist into Altium Designer. To import just a netlist, the netlist has to be in Protel format. HOWEVER, you can import the entire Orcad Schematic project into Altium Desginer. Once you've imported the schematic, and cleaned it up, you can generate your netlist directly in AD.
There are many very useful new features in AD6.8. The new 3D capabilities are very nice for those who use such things. However, it does take a good graphics card to handle the 3D displays - you have to have a fast card with DirectX 9.0c and Shader Level 3 capability. The 3D display puts a heavy load on the graphics chips. Most users will find that the graphics card runs hot when panning and rotating a PCB of any appreciable size. The really useful additions are in the schematic editor wiring harness, reusable schematic device sheets, enhanced library editing capabilities, etc.
I've got a problem with the DXP's design viewer. All the times when I import the drill files to this gerber viewer they are misplaced (look the example pic).
How could I solve this problem? If you want some points and have an idea, tell me!
This is not an Altium problem. Anyone who has worked with a CAM editor has seen something like this before.
You made two mistakes when importing your drill file into the CAM editor. First, you used the wrong setting for the number of decimal places when you imported your drill file into the editor - your drill display is several orders of magnitude larger than your board. Second, when you generated your Gerber and drill files you used relative instead of absolute origin - drill files are always generated to absolute origin. It's just the way the file formats are specified.
Once you import your drill file using the proper settings for the decimal places, you can move the drill layer to align with the other layers. There is an "Align Layers" menu item in the CAM editor.
This is not an @ltium problem. Anyone who has worked with a CAM editor has seen something like this before.
You made two mistakes when importing your drill file into the CAM editor. First, you used the wrong setting for the number of decimal places when you imported your drill file into the editor - your drill display is several orders of magnitude larger than your board. Second, when you generated your Gerber and drill files you used relative instead of absolute origin - drill files are always generated to absolute origin. It's just the way the file formats are specified.
Once you import your drill file using the proper settings for the decimal places, you can move the drill layer to align with the other layers. There is an "Align Layers" menu item in the CAM editor.
I saw the demos on altium and also I read the release note, lets discuss about these issues:
About wiring harness: I sense that it is just a graphic and luxury, and I can not understand what problem they were trying to solve?
Reusable schematic device sheets: exactly is the issue which I was looking for! Solving the reusing problem by other means and managing revisions and parameter was a big problem.
Enhanced library editing capabilities: would you explain it more? I do not notice it.
Here another question:
In AD can we have a parametric string on PCB or schematic? Suppose that you have a component which needs special care from fab or assembly, and you use the designator in string to describe it. But after annotating the designator will change and you have to re-edit you string. I am looking for the possibility of updating those strings automatically after annotating.
Also can we link office tools with our design files? I want this to automatically change the board documents after revision or any other board or schematic change!
After switching from AD to PADS and two month working with PADS, now I understand what you said about them in a comparison! Now I can repeat my experiences to other PCB designer: Do your job as much as possible in AD. For PADS users, AD is dreamland!
I am interested to know your opinion and comparison about PADS and Allegro, especially Allegro v16 and its new decoration?
Added after 1 hours 1 minutes:
Would you explain this issue in more detail: "relative instead of absolute origin"
I was supposing that, it does not matter to use relative or absolute origin for mask data generation!
The signal harness in AD6.8 allows you to group related signals together, similar to a bus. It simplifies the schematic. There is an online video that describes how to use it at: **broken link removed**.
In the schematic library editor, for example, you can now show and position the designator and comment strings for each of the symbols in your library. You can see some of the new features in the What's New PDF at: **broken link removed**
Yes, you can define parameters that will carry over to your schematics and PCB. You define them in the Project Options under the tab "Parameters".
No, you can't have office documents automatically updated by changes in the schematic or PCB.
Allegro is a more difficult program to learn and use than PADS. It also costs several times more than PADS for the same capabilities. The signal analysis and signal integrity tools that you can buy for Allegro are much better than tools available with other EDA packages.
The relaitive origin is the origin you set for your board. The absolute origin is the origin that your EDA software uses to define the limit of the workspace. If you use the same origin for Gerber and drill file generation, you will not have to manually align the drill and Gerber layers in a CAM editor. Several EDA programs automatically use absolute origin for drill files. If you use relative origin for the Gerber files, the drill and Gerber will not be automatically aligned when opened in a CAM editor. It's just a matter of being consistent when generating fab output. Anyone who is proficient with a CAM editor can compensate for alignment differences between relative and absolute origins; however, it's better to stay consistent.
Some one was talking about Expedition and Board Station, and claims that those two tools are superior to PADS; do you have experiences over these tools?
However I suggest, you may recommend me to stay with PADS and do not change to Allegro (?)
Currently I am using OrCAD + PADS; PADS is much faster than AD, but transferring netlist and ECO to PADS is very difficult. Also I saw very bad mistakes: net connection misplace!, it is not clear now who made this mistake. I am trying to replace OrCAD with DXDesigner. Another reason is that back annotating from PADS to OrCAD is not possible!
It seems that you were in this industry since many years ago, once you said from early days of starting Protel Company, so you have more than 20-year experience. Do you have your own company?
This is new for me:
**broken link removed**
I am not sure, but looks to be useful.
Expedition was purchased by Mentor from Veribest. I used the program when it was still owned by Veribest, and I liked it a lot. It had many very good features, and was relatively easy to use. The "Destination" autorouter in Veribest was far better than Mentor's router in PADS. I haven't used Expedition since Mentor bought it, so I can't comment on how good it is now.
I haven't used Board Station, so I can't compare it with PADS.
Unless you want to spend a lot of time learning how to get the best results out of Allegro, I don't recommend it. It is a powerful program when you combine it with the extra utilities you can buy for it. However, it is difficult to use. If you do take the time to learn Allegro, there are many companies who will pay well for your abilities. Some very large companies use Cadence products because their purchasing departments believed that the most expensive software must be the best. Once they invested hundreds of thousands of dollars they weren't going to just give up and throw the software away, so they stay on maintenance and continue to use the software even if it isn't the most efficient package available for their needs.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
