derived sketch does not update as it should

[JimmyDoe]

Hello all,

I am having some strange/bad behavior happening with derived sketches. I have a master skeleton and I am deriving it into a second skeleton, which only contains one sketch from my master. I am doing this because I am making a second small frame and only need one sketch from my master to use frame generator and don't want a hundred planes and sketches when all i need is one little sketch.

The problem is that when I change a plane, or add a line or make any modification to the sketch in my master skeleton my derived sketch will not update until I select 'Edit Derived Part' when I right click on it in the browser. The lightning bolt is not lit up, I hit rebuild all and nothing. All the little basic suggestions have been tried.

Is this just another thing in Inventor that doesn't work as it should?

[mdavis22569]

what version?  

Can you share it?

Also if you're on 2017, make sure you have the updates... If I recall correctly, there was an update that helped with the device command issues. 

[JimmyDoe]

I'm on Inventor 2016 SP1.

I'll see if I can attach the files, but for now I have attached a screenshot.

The blue sketch is the one in my trap door assembly, that has been derived from my main skeleton.

The white sketch is the sketch from my main skeleton, that the blue one is derived from. (they should match)

I have tried updating, rebuilding, editing the derived part. I can't figure it out.

[JimmyDoe]

I just restarted Inventor and now it updates on 'Rebuild All'

Does this not bother anyone else? That you must restart Inventor when you want changes to take place? How does anyone have ANY confidence when using Inventor?

This program seems to have more bugs than any other program I have ever used. It seems it's all just workarounds and mysteries.

[SBix26]

It certainly would bother me if I ever experienced anything like this, but I'm not seeing it.  I don't do derived skeletons, but I've currently got a pretty messy multi-body master part with some of its derived parts in a subassembly and others placed directly in the next higher-level assembly, and all I have to do is click the update button in the higher assembly and it all jumps into place.  I've even changed a few parameters in the master just to entertain myself, watching  everything adjust to the new geometry, then change it back again (I need to get out more...).

Sam B

Inventor Professional 2017 R2
Vault Basic 2017
Windows 7 Enterprise 64-bit, SP1

[blair]

It almost sounds like a previous version of Inventor didn't close properly or a file still had a lock on it. I really can't say that I have ever had this issue before.

Nothing like good old system reboots once a week, full power down and power up to keep everything fresh and clean.

[JimmyDoe]

I can guarantee that Inventor was closed properly, with all files closed and and then Inventor. All files had not even been checked into Vault yet. I have seen this behaviour on previous top down models. I fully shut down my computer and restart more than once a week. I've always had issues with Inventor not updating as it should, using derived skeletal sketches into 'sub-skeletons'. Is this a bad practice? And if so, can you explain a better way, so that I don't have hundreds of sketches and planes in my single assembly that contains 8 parts?(the reason for my multiple skeletons) It is just very frustrating and worrisome that I have to restart IV to get it to update as it should. Especially when other people don't seem to have this issue.

As for locked files; are you saying that I should always have all my models checked out?..since Inventor always asked to save files with no modifications anyway?... Just to be fully clear, what do you mean by locked? Released files?

I have read on here that if you derive a sketch you should create a new sketch in the derived model that just traces over the derived sketch. This doesn't seem to make sense, because my model did eventually update. But I'm just trying to find any straws to grasp at.

Does it help to purge my C: of all my old Vault files more often?

[blair]

When Inventor is editing a file, there is a "lock" placed on the file which is then released upon proper exit. Not to the extent that "Vault" does.

The exiting of Inventor and restarting seems to point in this direction, as all files should be closed when you close any application, all files should be closed and released.

Try using the "Close All" in Inventor and see if that solves your problem. Possibly with links to skeletal files, not all files are being properly closed.

The "Purge" function only deletes all old versions who's file status has been set to "Release" within the iProperties.

It's good practice to defrag your hard-drives on a regular basis. This will improve read-write performance as well.

[JimmyDoe]

I do close all of my open files before I close Inventor. But there is a button that will close them and ensure they are all closed properly? So, Inventor will be happy?

For purging Vault files, I mean deleting all the folders off of my C: that are already in Vault, and not modified on my machine.

[blair]

Yes there is:

[JimmyDoe]

Ok, thanks for the suggestions, Blair. I appreciate it!

[Anonymous]

Hi!

Experiencing the same problem but I see that no real solution was provided in this thread. Actually attempting to help a colleague with the same issue so I opened copies of the files on my station but can't manage to properly update the derived sketch either.

What do you suggest?

[JDMather]

---

@Anonymous wrote:

What do you suggest?

---

Attach sample files here that exhibit this behavior and end all doubt.

[Anonymous]

I had to purge a lot to be able to post the files but keep the primary sketches to show issue.

SKF2023 is the parent skeleton on which I drew a zigzag directly on the plan sketch just for the purpose of demonstration.

SKJ2023 is the base for a part in which references where derived. As you can see (or should see) the zigzag does not appear in part.

Looks like the sketch is locked in a certain version and cannot be overwritten. If I delete the derived skeleton and reinsert again I can see the zigzag but this is not a solution I can consider due to amount of features we would need to reattached. Those are not in the files I attached but know that the browser list is long.

Thanks for looking into this.

[blair]

You have your files mixed up. The "SKJ2023" is Derived from the "SKF2023" file. The "SKF2023" file has links Derived from the "683-Dies Layout.ipt file.

Start from the first part and work your way through.

[johnsonshiue]

Hi! I think this might have something to do with "DIES PLAN" sketch in SKF2023 is partially derived to SKJ2023. To be exact, only the sketch block SANDWICHPLATE @ 94:2 is derived. As a result, only the change in the block would trigger an update in SKJ2023. You will need to derive the whole sketch DIES PLAN to see the zigzag.

Thanks!

[Anonymous]

Hi!

In a way this makes sense but since the zigzag is not a block but directly drawn in the DIES PLAN sketch I'm surprise that some not useful block not being derived actually make a difference? We often work that way; the Dies Layout contains all the shapes required for our project and we derive only the required blocks when needed.

Thanks,

[JimmyDoe]

Hey!

I'm back. I left my workplace that used Creo to work with IV, then went back to the previous company that used Creo. Then I got a call from the employer that used IV so I'm back using IV.

Old habits die hard, in more ways than one. I'm having the exact same issue with a new completely brand new model.

I made a sketch of a slightly open circle to create a contour flange. I made a drawing for rolling purposes but now need to make it a 240 degree curve. I changed the sketch to be 240 degrees but the part stays the full circle.

This is the stuff that made me hate coming to IV from Creo and it feels like deja vu..

[johnsonshiue]

 Hi Nathan,

Welcome back! I know exactly what you are talking about. Inventor Derive paradigm is a surrogate/reference model. It is not a completely total derive. Some change in the source can propagate to derived objects but some don't. This is particularly true when there is topological change. For example, the line is split into two lines. Or, an open curve becomes closed.

We don't have a good solution to these behaviors yet.

Many thanks!

[JimmyDoe]

Ok, that's too bad. But thank you for letting me know that this is known behaviour. At least now I know I'm not just some really terrible designer of top down assemblies haha Thanks Johnson, keep crushing these bugs!