Passing parameters to an assembly?

[Anonymous]

I have a master layout (ipt), from which I've created derived parts, that get put together in an assembly. I'm able to pass parameters from my master part to the derived parts, but I don't seem to be able to pass parameters from the derived parts to the assy. Is this possible?

Thanks in advance,
Richard in Houston

[Anonymous]

One way to pass/share parameters to both parts and assemblies would be to use a linked (not embedded) spreadsheet. Blane

[Anonymous]

Yes it is. Open the parameters dialog in the assembly, and click link down at the bottom. Change the file type to .ipt, and select your master sketch file. It will link the parameters marked for export in your master sketch file... -- Cory McConnell Autodesk Inventor Certified Expert www.mechanixdesigns.com

[Anonymous]

Thanks for the replies.
I guess linking to the spreadsheet should have been obvious since my master sketch is driven by a spreadsheet. I did not realize I could link to the .ipt, which is ideal for this particular situation.

Thanks again,
Richard in Houston

[Anonymous]

Linked spreadsheets can become cumbersome if you ever need to rename or copy them for another application because renaming of excel file and OLE links cannot be updated using DA. This makes any changes in excel files more time consuming to update. Dont get me wrong tho if you have a unique application where excel filename is never changed it works fine.

[deltades]

I want to use I logic to adjust an assembly constraint based on T/F value passed from a master sketch. 

I have passed the paramater T/F and/or a user paramater as described in this thread using link (neet trick).. but when the code fires it only works on the true application and not the false.. if i open the rule and then close it the update button  becomes available and when updated the false condition updates sucessfully. I have tried just re-running the rule to no avail. It seams that the only way I can get it to triger a false condition is to open the rule... close it and update. 

any ideas?

[Curtis_Waguespack]

Hi deltades,

In the future feel free to start a new post and just add a link to this one for reference, rather than appending your new question to the existing thread. It's not a big issue either way, but you'll likely get a better response by doing it that way.

As for your question, I think we'll need to see your code, but you might try adding an Update line to your code to have it update the part.

InventorVb.DocumentUpdate()

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Edit I see you started a new post when I was typing:

http://forums.autodesk.com/t5/Autodesk-Inventor/assembly-constraints-driven-by-ilogic/td-p/3823803

If my suggestion works, please link your new thread to this one so others can find the solution in the future, otherwise just reply to your new thread.

[deltades]

I did.. should have started an new thread to begin with.. 

anyway .. see the code below

I added your suggestion but it didnt seem to help.. only if i open the editor and close it does it update.. very odd

Parameter("AC100-0100MRL-S:1", "iTrigger0101000") = 0 ul

If Parameter("iTrigger0101000") = 1 Then
d37_Header1 = -.25 in
d34_Header2 = -.25 in
ElseIf Parameter("iTrigger0101000") = 0 Then
d37_Header1 = -.25 in
d34_Header2 = 0.0 in
End If
InventorVb.DocumentUpdate()

[DRoam]

Hi, deltades. I would guess that since the rule works when you close the editor, what's actually happening is that the rule is simply not running when the "iTrigger0101000" parameter is changed. This is simply due to how iLogic works. To make the rule run automatically, my suggestion would be to open your "AC100-0100MRL-S" part and go to the Manage tab --> iLogic panel --> Event Triggers, right-click on "Any Model Parameter Change", and add your rule to this trigger, so that it will run each time any parameter in the part file is changed.

[deltades]

Ok.. question.. Are you  saying I can create the rule in the skeleton sketch and then push it up to the assembly?

Now that I think about it I think this can be done and it would improve the over all design.

Thanks!