Greetings!
The question I want to ask is about reference dimensions in iPart.
I can create a sketch and place reference dimensions on it, there's no problem. I can activate any configuration manually and see the reference dimensions adjusted according to configuration, no problem again.
I would like to know — is it possible to automatically populate column of the iPart table with reference dimension value, as it stands for each configuration?
I was able to find some solution for that, but it's not automatic. I can mark reference dimension of export, and add it as a column to the table, but I need to manually activate each configuration to populate the column with measured reference value. Not very good, because there can be very many configurations.
Any ideas as of how to automatically get complete list of reference dimensions values for each configuration of the iPart?
Great question. Will someone please address this issue. We are using Inventor 2012 and we are having the same problem with getting a reference dim to populate into the family table. We need this value for our production drawings.
Hi @esmith53,
As far as I know, this is still not possibly. Please see this improvement idea and lend your support to it:
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hi Guys,
I have to admit, this is the first time I heard about the request. The main reason why a reference parameter cannot be listed on the table is because it is incompatible with the concept of "Author Table."
The table dictates how iPart behaves. It looks like you are looking for a "Read-Only" column which can be driven by something else. The dependency model is a little bit complicated. Technically, it should be doable but the behavior can be confusing.
Depending on how you want to show it and how to consume this "reference dimension", there is a workaround I can think of. You can go to Parameters dialog and find reference parameter and check "Export" status. In this way, the parameter will be listed in Custom iProperties. Then you can add the iProperty to iPart table. The catch is that you will have to activate each member in order to capture the correct iProperties. Is this something useful?
Many thanks!
It's certainly not a perfect solution because it's very time intensive, especially when there are a lot of ipart rows.
The main goal here is to have an adaptive table in a drawing that gives key values that may not be part of the ipart table, but are still dimensions worth noting in a drawing that change when ipart rows change.
This probably isn't the place to suggest changes, but it never seems to work for me in the idea station. Having a way to mark dimensions in a drawing or in a ipart/assembly as dimensions for an adaptive table in a drawing is really important. Think for inspection as well. Right now, you can create inspection dimensions, but you have to manually build an inspection table and enter values manually. When they change, there is a large margin for error with manual checking.
I don't know if you've found a solution yet, but a sort of similar problem i've had is generating imember files for parts with a lot of configurations. I found the macro code below ( I apologize for not giving credit but I can't remember where I got it). I tried and it isn't a direct solution to your problem but it may be the start of one. A macro may be developed to cycle through all the configurations and accept the adjustment. I am not fluent enough to build that but maybe you, your team, or some other generous soul on these forums is. Sad that just about every solution we need is "just make an iLogic macro". Which is great and I'm thankful for that, but, I think self checkout at stores is a copout making me do the stores work. So... Anywho, see below.
InventorVb.DocumentUpdate() ThisDoc.Document.Rebuild() 'If it is an iPart If ThisDoc.Document.DocumentType = kPartDocumentObject Then Dim oDoc As PartDocument = ThisDoc.Document Dim oDef As PartComponentDefinition = oDoc.ComponentDefinition Dim oFactory As iPartFactory = oDef.iPartFactory Dim oRow As iPartTableRow For Each oRow In oFactory.TableRows oFactory.CreateMember(oRow) Next End If 'If it is an iAssembly If ThisDoc.Document.DocumentType = kAssemblyDocumentObject Then Dim oDoc As AssemblyDocument = ThisDoc.Document Dim oDef As AssemblyComponentDefinition = oDoc.ComponentDefinition Dim oFactory As iAssemblyFactory = oDef.iAssemblyFactory Dim oRow As iAssemblyTableRow For Each oRow In oFactory.TableRows oFactory.CreateMember(oRow) Next End If iLogicVb.UpdateWhenDone = True
@Anonymous
@johnsonshiue @esmith53 @Curtis_Waguespack @Anonymous
Hi! Many thanks for sharing the iLogic rule! My take on this is still the same as My prior reply #5. I have articulated the reason why such parameter cannot be added to the Author Table. The same applies to Model States.
Without using the rule, I guess the Custom iProperty approach is still the best bet.
Thanks again!
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