Multiple Same Footprint Name
Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=797
Printed Date: 25 Nov 2024 at 9:19pm
Topic: Multiple Same Footprint Name
Posted By: lalexman
Subject: Multiple Same Footprint Name
Date Posted: 11 Jan 2013 at 8:52am
|
Hi, I am trying to create a Vishay SC70 3 lead device. In the library I have there are 4 SOT210X110-3 Footprints. They each vary in some of the dimensions. I realize we have been down this path but I have a few questions. 1. Shouldn't they have a different name or at least a -1 -2 -3 -4 at the end to distinguish between footprints? 2. If I Build a library do I get multiple entires for these different footprints? 3. If multiple footprints are created does the footprint name change?
|
Replies:
Posted By: Tom H
Date Posted: 11 Jan 2013 at 9:06am
|
The component Package Height normally discriminates footprint names for the same package. What I do is create a full FPX file with these attributes - 1. Standard Component Family ID 2. Mfr. Component Dimensions 3. IPC-7351 Footprint Name 4. IPC-7351 Physical Description 5. Mfr. Package Case Code 6. Mfr. Name 7. Mfr. Part Number 8. Mfr. Logical Description 9. Mfr. Datasheet Link |
Posted By: lalexman
Date Posted: 11 Jan 2013 at 9:21am
|
Thanks Tom, For me personally I do not like the height in the decal because that causes you to create many decals that are basically the same decal(for example resistors) and using the height to determine the package is correct is not fullproof.Would it be possible in the future to have the capability to automatically add additional information to the footprint name like you did with the terminal size ? This would make it much easier to just look at the footprint name to determine if its the correct footprint ? Also can you please look at item two from my pevious post about building the library. Thanks
|
Posted By: Tom H
Date Posted: 11 Jan 2013 at 9:29am
|
If you build a library and many manufacturer's create the same package, I make duplicates in the FPX library because I like to track every part I use by every manufacturer. The Batch Build feature will only create 1 of each footprint name even if you have 1,000 identical footprint names. It's called Profesional Library Management. Plus you get the benefit of searching for specific mfr. case codes or part numbers to quickly locate parts that you already built. Build it once, build it right and never build it again. |
Posted By: lalexman
Date Posted: 12 Jan 2013 at 6:54am
|
Hi Tom, In the above example I provided I used the FPE library you sent me to look for the SC70 part. There are four footprints with the same name but different parameters . Based on your last statement , when the the library is built there will only be one of the four footprints in the library ? |
Posted By: kwgilpin
Date Posted: 18 Jan 2013 at 8:44am
|
Hi Tom, I'd like to resurrect this thread. You suggest adding a _TL* or _TW* identifier to the end of otherwise identical package names to differentiate them. When I do that, all is great until I select "Tools -> Regenerate Library -> Names". As a result of that operation, FPE removes any custom suffix that I have assigned to a part's footprint name. Any suggestions for a work-around? Will you consider changing the code so that all part name suffixes beginning with an underscore are left in place when regenerating names? Thanks, Kyle |
Posted By: Tom H
Date Posted: 18 Jan 2013 at 8:52am
|
There
are hundreds of footprints that have the same identical name with different
tolerances and thermal pad sizes. The FPE FPX file is intended to be used as a
library source for users to quickly locate the correct component package data
row and copy/paste that row from FPE FPX into your personal library. When doing
so, it’s up to you the user to rename the footprint to avoid duplicate
footprint names with tolerance and thermal pad differences. There
is no guidance from IPC at this time on how to handle variations in Thermal Tab
sizes. One of the recommendations PCB Libraries, Inc. has for various thermal
pad sizes is to append the end of the footprint name with underscore _ and “T” (for Thermal) and the component Tab
Size. Examples: QFN50P600X600X100-41 rename to QFN50P600X600X100-41_T365 = Thermal Tab size is 3.65 mm square QFN50P600X600X100-41_T365X200 = Thermal Tab size is 3.65 mm X 2.00 mm rectangular Using this technique will eliminate duplicate
footprint names with various Thermal Tab sizes. There are also variances in the Lead
Tolerance that will produce a different footprint pattern pad size and spacing
with the same footprint name. There is no guidance from IPC at this time on
how to handle variations in Lead Tolerances sizes. One of the recommendations
PCB Libraries, Inc. has for various Lead sizes is to append the end of the
footprint name with underscore _ and “L”
(for Lead) and the component Lead Size. Examples: SOP65P490X110-8 rename toSOP65P490X110-8_L38X68 = Lead size is 0.38 mm minimum and 0.68 mm maximum We
have narrowed land pattern name duplication problems down to 2 areas. 1. Thermal Pad
Sizes - _T350 = Thermal 3.50 mm Square or _T350X200 = Thermal
3.50 mm X 2.00 mm Rectangle 2. Lead tolerance
- _L38X65 = Lead tolerance is 0.38 mm X 0.65 mm If
we add a radio button into component families that support Thermal Pads to
append the end of a footprint name to add #1 then that would be the
differentiator and make every footprint name unique for those parts – QFN,
PQFN, SON, PSON, SOP, QFP. If
we add a radio button to all Gull Wing lead component families to append the
footprint name with the Lead tolerance, that would differentiate all duplicates
in the Gull Wing parts for SOP, SOIC, QFP, SOD, SOT, TO, etc. With a Radio
Button, users can turn this feature on/off as needed. We are lobbying IPC to add this to the next
release of the IPC-7351C standard. |
Posted By: lalexman
Date Posted: 18 Jan 2013 at 8:54am
|
Hi Kyle and Tom, I like your idea Kyle or perhaps an option to all any of the additional parameters to be added to the footprint name. I understand your point Tom that at one point all the parts will already created but here is my problem. I have a new 4 pin smt oscillator. I look thru my library that the decal name has body size, pad size and pad pin to pin pitch in x and y. I can easily see if I have a decal that matches by looking at the name. I did not so I go to the Footprint expert . The footprint name does not have all the needed info so I have to load each footprint to see if one is the same.(Yes I know I can look at the manufacturer name and package but this OSC did not exist there either). The height in the name does not help since the part is a different height. Having more info in the footprint name will make it easier to find matching footprints IMHO. |
Posted By: kwgilpin
Date Posted: 18 Jan 2013 at 9:02am
|
Hi Tom, Thank you, as always, for your blazingly fast responses. I really like your proposal, and I'm excited to see it implemented as soon as possible. Along with what you propose, one other option, that I think would make many people (including myself) even happier would be to add a "custom suffix" column to the library templates. Whatever is in that column would be appended with an underscore to the very end of the footprint name. My impression is that there are many users who want a little more flexibility in naming than what the IPC provides. These options would certainly give it to them. |
Posted By: Tom H
Date Posted: 18 Jan 2013 at 9:17am
|
Are you referring to a new Column in the FPX file? Normally I add a "Notes" column and I add everything special that I did to create the library part. I especially keep a separate FPX file for every part when I use the mfr. recommended footprint feature so that I know that those parts do not use the standard Preference DAT files. |
Posted By: kwgilpin
Date Posted: 18 Jan 2013 at 9:21am
|
Yes, a new column in the FPX file titled "part name suffix". The "part name suffix" column would be unique (i.e. different from your Notes column) because FPE would automatically append its contents to the end of the part name. This solves the problem of user-generated suffixes being deleted when you regenerate the library names. Does that make sense? |
Posted By: Tom H
Date Posted: 18 Jan 2013 at 9:28am
|
Yes, it makes sense, but when the user selects the Radio Button for "Add Thermal Tab to Footprint Name" that suffix will automatically be transferred to the FPX file "Footprint Name" column. It's automatic. When you create a single part or batch build the entire FPX file the new suffix will be in the name. I'm seriously considering updating all of our QFN, SON footprint names to add the Thermal Tab suffix once the new radio button is implemented. Then I can do a "Tools > Regenrate > Footprint Name" and it's automatic. |
Posted By: lalexman
Date Posted: 19 Jan 2013 at 4:34am
| Is it possible have that Radio button include the other parameters that you have discussed above ? |
Posted By: Tom H
Date Posted: 19 Jan 2013 at 9:37am
|
Let me explain... In the V2013 release there will be 2 new on/off Radio Buttons for -
QFN Examples of adding Thermal Tab data: QFN50P600X600X100-41 rename toQFN50P600X600X100-41_T365 = Thermal Tab size is 3.65 mm square QFN50P600X600X100-41_T365X200 = Thermal Tab size is 3.65 mm X 2.00 mm rectangular SOP Examples for Lead tolerance data: SOP65P490X110-8 rename to SOP65P490X110-8_L38X68 = Lead size is 0.38 mm minimum and 0.68 mm What other Radio buttons do you want (specifically list them for our programmers)? |
Posted By: lalexman
Date Posted: 19 Jan 2013 at 10:16am
|
Body Size max (x and y) on any device, lead size Max(x and y) on any device, Lead distance end to end on any device that the leads are larger then the body, bga pad size, DFN pad center to center spacing. Basically what I am looking for is enough info in the footprint name to see quickly if the footprint matches the manufacturers device spec. |
Posted By: Tom H
Date Posted: 19 Jan 2013 at 10:33am
|
Unfortunately, IPC only recommends footprint names to be created with elements that solder to the PCB. The Lead Span, Pin Pitch, Pin Qty, Lead Width & Length, Ball Size, Thermal Tab size, Lead tolerance. The only exceptions to this rule is the component Height becasue it affects the 3D model name and BGA because Memory Chips have the same package size for various memory limits, 4GB, 8GB, 16GB, 32GB, etc. i.e.: there is not any component package dimensions in the IPC naming convention. IPC approved the to add the Thermal Tab and Lead tolerance suffix extensions as optional data to reduce duplication. The User can easily edit the Footprint name in the FPX file to whatever you want. It only takes a couple seconds to add any additional data to create customized footprint names. The future feature modules the "Package Editor" and "Footprint Editor" will have custom footprint names that will apply to 50% of all packages in the industry. Example: Component Family _ Mfr. Name _ Mfr. Part Number This does not include any component package dimensions and there are no duplicate footprint names. Maybe every footprint name should follow this non-standard package convention as component manufacturers are producing non-standard parts.
|
Posted By: lalexman
Date Posted: 19 Jan 2013 at 10:57am
|
So it sounds like are you saying you can add everything I suggested except body size ? I realize you want to be IPC compatable but why is adding an option to a name we the users might need a problem ? Yes we can add it to the FPX file but that does not work in batch mode and adds more time to creating a footprint.
|
Posted By: Tom H
Date Posted: 19 Jan 2013 at 11:03am
|
Manually changing (customizing) the Footprint Name in the FPX file works perfect in Batch Mode. There are too many people who want too many different customized options to add to the program GUI. This makes the User friendly GUI and makes it complicated. |
Posted By: lalexman
Date Posted: 19 Jan 2013 at 11:09am
|
You asked "What other Radio buttons do you want (specifically list them for our programmers)? I responded to ones I though you could add based on your statement plus the body size that is not IPC approved and you cannot add. So you are not going to add any other options to the radio button then the two you mentioned above ? |
Posted By: kwgilpin
Date Posted: 19 Jan 2013 at 1:04pm
Hi Tom,
This isn't entirely true. As soon as you select "Tools -> Regenerate Library -> Names" from the menu system, all custom names are destroyed. This is why I was suggesting a new "Part Name Suffix" column be added to the FPX databases. When told to regenerate names, FPE would attach the contents of this column to each part name. |
Tom H wrote:Posted By: Tom H
Date Posted: 19 Jan 2013 at 1:06pm
|
I see your point. We'll have to consider this in the V2013 release coming out on February 1. |
Posted By: kwgilpin
Date Posted: 19 Jan 2013 at 1:11pm
| Thanks Tom. I'm looking forward to it. |
Posted By: Dale
Date Posted: 20 Jan 2013 at 3:30pm
|
In Expedition's padstack generator the hole names and pad names are automatically generated based on their physical attributes. However in front of each name (in a list view) is a tick box which is labelled "Generate name from properties". If one deselects this box, the autogenerated name remains but then one is free to edit it in any way. I have found this mechanism to be very effective and would recommend considering it for your footprint names. I will also give my vote to a separate Suffix field which is always added to the end of any autogenerated name. Regardless of how good the autogenerated name is, there will always be times when a non-standard suffix makes sense. |