There isn't an option to do this, the properties get 'promoted' as you edit them or change visibility.
Robert, if this is the case, is there a way to change component attribute in the drawing, and to prevent library data override lateron (on current board)?
What is the process you are doing here? What are the reasons for updating the symbol?
In case of any change in the library sumbol, I am interested in the sumbol update, however, I dont want it to change the component value and mfg. part number which I defined for the specific board.
In addition, there is a problem with the attribute label location: if I move it because of current drawing needs, while updating a symbol for the central library, it will be relocated. It cause a waist of time
to re-arrange all labels.
Updating the symbol won't override changes made on the schematic, the block or instance value will override the symbol value. Similalrly it won't move the properties from their current location, to set them back to symbol default you need to run the Reposition Properties command.
I investigated this issue to define exactly my problem. Robert, please explain what is the "symbol attribute value" vs "block attribute value"
I did not have it in old DxD versions. How can I define which of them will be shown in the partlist excel file?
It looks that I change the component value in the drawing, but the library value override it and appears in the excel. TIA
There are three 'levels' of property, Symbol, Block and Instance. Symbol is the value defined in the symbol file, if there is one rather than just a placeholder. Block and Instance are schematic level properties, if you modify a symbol value by changing the visibility or assigning a different value it becomes a block value. If the schematic were a hierarchical block and was used more than once in your design then all instances of the block see the same value. Where a property is required to be unique in a design, say a Reference Designator, then it gets assigned an 'instance' value. For a repeated hierarchical block you would see the instance value in each 'instance' of the block.
The concept is not new, you had symbol, block=promoted and OATS in earlier versions, it is more exposed in the newer versions of the software.
My tests with part lister do not exhibit what you say you are seeing.
I have a capacitor with a Value=200 defined in the symbol. Place this in the schematic and the part lister lists the value as 200. Change the value to 300, the property dialog indicates a symbol value of 200, block value of 300, part lister outputs 300. Add an instance of 500 and 500 is output to the part lister.
You don't say what version you are running of the software.
Sorry Robert, it took me time to understand what really wrong.
I have to give an example to clarify the case:
Please follow this process:
1) I import from central library 1uF capacitor.
2) This is a library capacitor has it's MFG attribute and MFG_PN attribute.
3) I need in the drawing 2uF capacitor too. So I take the 1uF cap, copy&paste it on the drawing
, change its value to 2uF and erase the MFG and MFG_PN
3) I run netlister
4) Netlister put the 2uF in a separate line, but it got the MFG and MFG_PN from the 1uF cap, as it looks on the capacitors as the same component.
What is the correct process to prevent suct incident?
The proper procedure is to create a new 2uF part in the library, and add that part to the design. Then every time the part is added from the library it will be consistent with the data entered from the library. In your case, the Part Number property stll specifies the 1uF part and therefore the 1uF properties are added to part instance when packager is activated.
Thanks Gary, but it means that I have to create a library component for each cap value?
it is not reasonable, I don't understand why I had no problem with it using DxD 2005, and I am using
Viewdraw for 10 years.
Gary, I am looking for a way to define which attribute will be domained by library value, and which by drawing value.
Is it possible? I face very strane cases in 9.5 like: I have components in the drawing that I can't change their attribute.
Is there a document which discribe specifically this issue?
You can use a generic capacitor and asign the DEVICE (or your choice of part number property), PKG_TYPE & VALUE properties (and any others you want) at the schematic level. Just as you did in the older versions of DxDesigner.
The inability to change properties on a component is caused by non-common properties. TechNote mg511904: a Non Common Property to a Common Property has a script that will help you make the conversions so you can edit the properties on your components.
Thank you all for your support. I'll re-orgenize the library components to solve this issue, no easy way to do it...