Updating entire assembly using iLogic

[Anonymous]

Hi All,

Having a few troubles updating and saving a couple of iLogic controlled assemblies i'm working on...

Firstly, i want to perform and update and save of the main assembly before triggering the opening of the various IDW files to save as PDF's. 

The only 2 functions i currently know of are:

InventorVb.DocumentUpdate()

&

iLogicVb.UpdateWhenDone = True

It seems that InventorVb.DocumentUpdate() doesn't seem to perform a proper "update" in Inventor terms as the geometry is not updating immediately and the update button in Inventor is still active after running the rule using this method.

The iLogicVb.UpdateWhenDone = True works perfectly, the only problem is that if i trigger another rule or perform other functions within the rule containing this function, the resulting drawings aren't updated as the update doesn't complete until after all the rules have finished running (a little pointless in this scenario).

The overall aim is to completely update and save (in order to update BOM) the top level assembly, and then subsequently trigger the opening of the relevant 2D drawings. I have figured out the launching, save as, and closing of the 2D drawing files, but i can't seem to get the information updated and saved before it all happens!

Any advice is appreciated...

[MjDeck]

If you're not already doing it, try using this sequence:

RuleParametersOutput()

InventorVb.DocumentUpdate()

RuleParametersOutput() is required if you have changed parameter values directly by assigning values to them in the rule.  These changes won't be propagated to Inventor until you use this function (or the rule finishes running).

[Anonymous]

Thanks Mike, that extra line works a treat at the assembly level.

My next problem is that in the drawing file that is opened, all of the information in the parts list, title block etc is updated, however the drawing views are not updating correctly. There are no updates pending, and if you highlight the entire drawing view using window select, it appears that the correct updated view is "invisible" in the background with the previously saved view sitting there in front.

Any suggestions why this might be happening and / or are there any additional lines of code to force a complete update on all drawing views?

Thanks,

[MjDeck]

What version of Inventor are you using?

Are the drawing views showing an assembly Level of Detail (not the Master LOD)?  In that case there might be trouble with iLogic rules that run on the After Open Document event in either the assembly or the drawing.  Do you have any rules that are set to run on that event.

[Anonymous]

I'm using Pro 2011.

Because i'm using component suppression, i have the assembly and sub-assemblies in "iLogic" LOD and this is reflected in the drawing views.

Also, both the main rule in the assembly and the main rule in the drawing file are both triggered to run After Open Document...

What is the known issue and how do we work around it?

Cheers.

[MjDeck]

The drawing has to open the assembly custom LOD for the views, but it also opens the Master LOD for the parts list.   This causes a conflict between iLogic rules and view update on document open.  We are working on a solution.

 To work around this problem, add these lines at the top of all your assembly rules that run on the After Document Open event, or that use the Component.IsActive function:

Dim doc as AssemblyDocument = ThisDoc.Document
If doc.ComponentDefinition.RepresentationsManager.ActiveLevelOfDetailRepresentation.LevelOfDetail = LevelOfDetailEnum.kMasterLevelOfDetail  Then Return

If (Not (doc Is ThisApplication.ActiveDocument)) Then Return

This will prevent the rule from running in the Master LOD, and it will also prevent it from running if the assembly was opened from the drawing.

 You also might have to avoid opening the drawing and the assembly in separate windows at the same time.  I would recommend making changes in the assembly without the drawing open, save and close the assembly, then open the drawing by itself.

[Anonymous]

Ahh i see!

What I need to do is open the main assembly which triggers the linking to a unique xls file, updates the model and saves (in an iLogic LOD) and then opens 3 drawings (one after the other is fine), updates the views and adjusts the view scales and positions, saves as pdf and then closes.

I have the main assembly working well (after the updates in your first reply - thanks!) and the triggering of the drawing to open, as well as the view scale, position and save as pdf all work well. The only issue is the updating of the drawing views upon opening the drawing file...

Is it possible to run the open / update / save as / close operations on the 3 drawings from a rule in the main assembly and have the main assembly close(d)?

[MjDeck]

If you want to automate the whole process, I would recommend putting the top-level rule in another document (not the main assembly) or in an external rule or external program.  Have the top level rule

- open the assembly (which will update by itself)

- close the assembly

- open each drawing (which will update and save as PDF)

- close each drawing

[MjDeck]

You might also have to remove the drawing rule(s) from the list of rules to run on the After Open Document event.  There might be a conflict with the view update.

[Anonymous]

Hi Mike,

It seems that the extra few lines of code you suggested to place into the top level rule to stop the changes running on the Master LOD have caused some serious stability issues in the rest of my model. A bunch of features are not changing or updating as they did previously. I've commented out the lines to return it to the previous state and they're working fine again. Looks like i'll have to attack it in another way...

Do you know if the issues mentioned are being addressed for 2012 release?

[MjDeck]

Andrew,

 I'm not sure exactly what's causing the problems.  If you can upload the model or get it to me by email or Buzzsaw, then I can take a look at it and test it.

 Note that saving (or saving as) the model within a rule that's within the same model doesn't always work.

In a previous reply I recommended:

If you want to automate the whole process, I would recommend putting the top-level rule in another document (not the main assembly) or in an external rule or external program.  Have the top level rule

- open the assembly (which will update by itself)

- close the assembly

- open each drawing (which will update and save as PDF)

- close each drawing

Did you try that?