USE DISCOUNT CODEEXPERT30TO SAVE $30 USD
Altium Clearance Matrix Itnterpretation
Diva , 03-30-2022, 11:59 PM
Hi All I would like to know how do you interpret the Altium Clearance Matrix.
I know that the clearance is between any two objects kinds and there are many in Altium such as tracks pads vias etc.
There is the first object matches field and similarly the second object matches field to specify the objects to be checked for clearance.
What I am not clear is the following.
Does the ROWS of the Clearance Matrix is associated with the First Object Field while the COLUMNS are associated with Second Object Field.?
Alternatively is it reversed that is COLUMNS are associated with First Object Field and ROWS are associated with the Second Object Field.?
Or my understanding of the Clearance Matrix is wrong?
Regards
Diva
I know that the clearance is between any two objects kinds and there are many in Altium such as tracks pads vias etc.
There is the first object matches field and similarly the second object matches field to specify the objects to be checked for clearance.
What I am not clear is the following.
Does the ROWS of the Clearance Matrix is associated with the First Object Field while the COLUMNS are associated with Second Object Field.?
Alternatively is it reversed that is COLUMNS are associated with First Object Field and ROWS are associated with the Second Object Field.?
Or my understanding of the Clearance Matrix is wrong?
Regards
Diva
qdrives , 03-31-2022, 08:03 AM
The first and second object are the kind where to compare against. I mostly use net classes in these.
The matrix is used to set the clearance depending on the type. Often, this is just simply a single value.
Examples:
48V power nets - First object: In netclass('48V'), second object: all
Matrix:
minimum clearance: 0.25mm
TH pad (to all): 0.6mm
Other selections for the objects are layer and rooms.
For some clearance values: https://www.frontdoor.biz/PCBportal/clearance.gif
The matrix is used to set the clearance depending on the type. Often, this is just simply a single value.
Examples:
48V power nets - First object: In netclass('48V'), second object: all
Matrix:
minimum clearance: 0.25mm
TH pad (to all): 0.6mm
Other selections for the objects are layer and rooms.
For some clearance values: https://www.frontdoor.biz/PCBportal/clearance.gif
WhoKnewKnows , 03-31-2022, 08:36 PM
Diva, it might be satisfying to know, but I suspect it doesn't matter. I saw this post earlier today and have been thinking about it.
Say the first drives all of the columns and the second drives all of the rows. The first has all of the possible different types of objects represented and the second has all of the possible different types of objects represented. Would you put a different clearance for the first's via against the seconds track than the first's track against the second's via? Anyway, perhaps I'm not thinking of all of the possible ways this could bite the user.
Say the first drives all of the columns and the second drives all of the rows. The first has all of the possible different types of objects represented and the second has all of the possible different types of objects represented. Would you put a different clearance for the first's via against the seconds track than the first's track against the second's via? Anyway, perhaps I'm not thinking of all of the possible ways this could bite the user.
qdrives , 04-01-2022, 09:58 AM
@WhoKnewKnows No, the first/second object do NOT drive the rows/colums.
Take a look at the screen capture below.
In the red 'circle' are all the clearances for a TH pad compared to all the other items (including other TH pads).
In the green areas are the first and second objects.
In this example I want:
1) The inner layers. multi-layer is mentioned explicitly as I also need via to via clearance on the inner layers. Altium has vias and TH pads only on multi-layer and not top/bottom and inner layers.
2) Compared to - well, everything is ok as we cannot compare clearance between layers. Keep it simple!
3) For the inner layers I want 0.25 minimum clearance. So just fill in 0.25mm in the minimum clearance box (not highlighted).
4) As standard for "different nets only"
You need multiple clearance rules when you are working with higher voltages (24, 48, 110(dc), 230, etc.).
You want to use the matrix when you want to differentiate the clearance for example polygons vs TH Pads and SMD pads (polygons are not shown in "simple").
Take a look at the screen capture below.
In the red 'circle' are all the clearances for a TH pad compared to all the other items (including other TH pads).
In the green areas are the first and second objects.
In this example I want:
1) The inner layers. multi-layer is mentioned explicitly as I also need via to via clearance on the inner layers. Altium has vias and TH pads only on multi-layer and not top/bottom and inner layers.
2) Compared to - well, everything is ok as we cannot compare clearance between layers. Keep it simple!
3) For the inner layers I want 0.25 minimum clearance. So just fill in 0.25mm in the minimum clearance box (not highlighted).
4) As standard for "different nets only"
You need multiple clearance rules when you are working with higher voltages (24, 48, 110(dc), 230, etc.).
You want to use the matrix when you want to differentiate the clearance for example polygons vs TH Pads and SMD pads (polygons are not shown in "simple").
robertferanec , 04-04-2022, 05:07 AM
I would not say there is a first or second object, these rules are just between two objects. Notice the empty cells - these are there to eliminate duplication of the rule in the "opposite direction".
Use our interactive Discord forum to reply or ask new questions.