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Parameters not updating

21 REPLIES 21
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Message 1 of 22
Scott_Stubbington
2470 Views, 21 Replies

Parameters not updating

Hello, 🙂

I have found a couple of times now a  problem with Parameters not updating correctly.  Last Tuesday (26/06/2012) I logged a call with the VAR and they are yet to contact me about the problem.  In the past when I found the same thing, a different VAR made excuses about not using the most current software as I developed the model on IV2010.  The Parametric model made use of VBA and Skeletal modelling and the VAR made excuses along the lines of we weren't running the most current software, didn't make use of iLogic and since I was using VBA and did not pay for the code checking service the problem for them disappeared as they were going to do no more.   When we finally upgraded to IV2012 and the problem still existed they consequently chose the excuse of my VBA code being the problem, consequently I then created a simple rule in iLogic and demonstrated the problem that way.  I lost my job with the company just as it looked as though the problem would be finally dealt with as it was forwarded to member of Autodesk UK.

To summarise, the model is a Parametric Skeletal assembly, it utilises VBA for a user interface.  The problem existed in IV2010, IV2011, IV2012 and IV2013.  There are pictures attached to show the problem.

 

Please please please fix the problem.

21 REPLIES 21
Message 2 of 22

I haven't come across this before. Maybe add your files so we can take a look to try to reproduce.
Message 3 of 22

Unfortunatley the data isn't mine to go leaving on the Internet.

Message 4 of 22

Then unfortunately it is hard to give you an answer without data. Make a small sample and send it.
Message 5 of 22

Thanks for your input, however I'm struggling to work out what answer you will give other than what I already know, if you want to check I am using Inventor correctly then please point this out to me.  If I could create a small sample I would, but I cannot sit here and say do this, do that and you will now have parameters that will not update.

Have a look at 20120705-SmallSample, this is the amount of formulas I will enter before I get to this problem, this isn't something you quickly rustle up.

Message 6 of 22

I've seen this problem before. It doesn't have anything to do with how many or how complex your parameters are. The problem that I see is the way that Inventor updates driven dimensions.

Try doing a rebuild all and see if that allows the calculations to come out correctly. If that works then you can use some iLogic code to make Inventor do the rebuild automatically.

Mike (not Matt) Rattray

Message 7 of 22

I believe I will try your suggestion, not too sure I haven't already, but to be sure I will give your suggestion a go.

 

Thank you 🙂

Message 8 of 22

Rebuilding the file didn't work so I tried rebuilding each file 15 times, that didn't work either.

Message 9 of 22

The thing is, if I edit the Master Part document directly (not via macro or iLogic) the correct values get flushed through.

 

See attached.

 

Where the picture states, "see post", if I disect the equation either side of the "+" symbol, the equation will correct itself.

Message 10 of 22

What does "Sign" = ?

Message 11 of 22

It would be really helpful if you could post files. Otherwise, we're just shooting in the dark.

Mike (not Matt) Rattray

Message 12 of 22

The Sign function returns either a 1 or 0, 1 if the number is positive or 0 if negative.   Udaya wrote a paper a while ago describing how to use the Sign function to create "If" and "Select Case" statements without using VB code.

 

http://www.mcadforums.com/forums/viewtopic.php?t=5536

 

I have a dataset, no macro.  I'm no good with iLogic so you will have to create your own rule to edit the Height and Width in order to recreate the problem, run the rule when you have the drawing open as this is where I would run the macro from.  The parameter problem is in the file LidProfile.ipt.

 

The rule.... in words....

The rectangular hole has a window placed on the underside of the plate, below the window on the top of the plate sits a label, there are two holes for fasteneing the label.  If the container isn't big enough to have the window on the centreline of the plate with the label below, move the window and label up.

 

"The attachment file size is too large. The maximum file size is: 1,572,864 bytes", attachment is 13 MB

Message 13 of 22

Did you try rolling up the EOP markers to reduce the file sizes?

Mike (not Matt) Rattray

Message 14 of 22

No I didn't move the EOP.  I moved the EOP and it's still too large.

Message 15 of 22

Try this, if it works they won't be there for long, if not, I'm open to other ideas.

 

https://skydrive.live.com/redir?resid=489CD8B53ADD9DF2!150

Message 16 of 22

I was able to download it, but I don't see anything wrong with it. Can you point me to where the error occurs.

Mike (not Matt) Rattray

Message 17 of 22

Are you able to create a simple iLogic rule to modify the design from the drawing document.  In the master part, there are three parameters, EnclosureHeight, EnclosureWidth and EnclosureDepth, these Parameters control the size of the Enclosure, focus a rule on changing the Height or Width.  The previous post 07-09-12 03:25 details the rule and if you are able to create an iLogic rule then it should become apparent.

 

Sorry for the lack of iLogic experience and thanks for your help.

Message 18 of 22

I've managed to create a simple rule in the assembly file.  If you would like me to upload a copy, let me know.

 

The Parameter to focus on is EnclosureWidth.

Message 19 of 22

It looks like my original theory was correct. I think you misundestood me, however. Rebuilding the model will only cause the paameter to update that one time. You needed to create an iLogic rule to force the model to rebuild everytime it's parameters change.

I added two rules to two of your files and this seems to have solved the issue with the sight glass cut out and tag not updating correctly.

 

In the "LidProfile" part I created a rule named Rule0 and added the following code to it:

InventorVb.DocumentUpdate(False)
ThisDoc.Document.rebuild
InventorVb.DocumentUpdate()

 In the top level assembly file, "Enclosure" I created another rule with this code in it:

InventorVb.DocumentUpdate(False)
iLogicVb.RunRule("LidProfile:1", "Rule0")
InventorVb.DocumentUpdate()

 

You can then go to Manage > iLogic > Event Triggers and set the assembly level rule to run on "Any Parameter Change". This will force everything to update correctly when you click update.

Mike (not Matt) Rattray

Message 20 of 22

OK, did that, works.

 

I cannot make LidProfile.ipt update correctly without iLogic, any attempt to Rebuild manually does not produce the required layout.  I pasted the iLogic code into the required rules and the part now updates correctly.

 

Many thanks. Smiley Happy

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