Assembly constraints gone wild

[Anonymous]

Hi everybody, I've been using inventor since series 9 and early on developed what I thouhght were good part creation habits. I always center the part on the origin point because this makes assembly models easier to assemble. Some of my models are pretty big, so i create sub-assemblies of the major elements, sides, floors, tail gates, bulkheads, suspensions and chassis'. (we manufacture trailer and truck bodies and chassis). So my problem is that sometimes when I open an assembly file to make a change or add a new part or sub-assembly, Inventor seems to have lost track of parts or assembly constraints and the model looks like it exploded, and I get the infamous red cross or error messages out the wazoo. At this point the model is pretty useless. Even when I open some of the sub-assemblies, they have "exploded" as well.

      I have a pretty simple file structure. I have a master "project" folder named Project. under that, are all my indivudual customer folders. Common parts are in a part library that is included in the project search path. I am the lone user of inventor, only one workstation, and not using vault. All my project files are stored on a server partition that only I use. (same drive, unique path)

                 Can anyone tell me how to prevent this from happening, or what causes it to happen. Or is this just on of those Inventor gremlins that everyone has to deal with some time. Any and all help appreciated. Thanks in advance.

                                       Frank

[mdavis22569]

Are you using IPJ's

[blair]

Odd indeed, sounds like you are using a simple Project File without to many libraries and folders. I might try copying the folders to your local machine and create a new Project File for the new location. Possibly a slow network might be causing issues with Inventor and timing when loading your model.

Keeping the Hard-Drives defragmented may help as well.

[johnsonshiue]

Hi! Frank,

Is that possible some of the geometry used to participate in constraints are gone or the components are gone? Could you post the example here or send it to me directly (johnson.shiue@autodesk.com)? I would like to take a look and understand the behavior better.

Many thanks!

[Anonymous]

Johnson,

I can't post anything at this time, but to answer some of your questions,
there should be no missing geometry or components. The assembly file just
seems to lose constraints or lose track of them. I usually have to go back
and delete unresolved constraints and re-apply them. If I do a component
replace (usually to use a unique part name for a left and right part) I
"save copy as" for a left and right part, then do the component replace. The
parts are the same geometry as the one replaced, just a different name.
Inventor seems to have a problem with this sometimes, then other times it's
no problem. Very inconsistent. If I start to have issues placing constraints
in an assembly file, such as getting the "place constraint" tool can't find
the constraining surface, even though the little arrow indicator is on the
surface, I find restarting Inventor clears up that kind of problem. I often
have multiple files open when this occurs (5-10 files) for the purpose of
comparison.



System specs.

Intel Core i7-3770 CPU@3.4GHz

RAM = 16GB

Windows 7Pro SP1 64 bit

ATIFirePro V7800 w/2G DDR5

Dual ASUS 27" connected via HDMI

2T HD











Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[Anonymous]

Mdavis,

I'm sure I have Inventor configured correctly, as least as
far as the individual project folders. I also have my common parts pathed
through the "library" option in the project configuration step when I create
a new project folder for new customer, if that's what your asking.



Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[Anonymous]

Blair,

Thanks for the input. I do keep as much local as possible
like the content center files (inventor still loses track of those). Not too
many Library paths, 2 I think for most projects. Not using vault as this is
a single seat, single user setup. Owner wants all CADD files on server for
security/backup reasons and also takes care of server maintenance (defrags).
I had tried at one point to move all currently active files to my local
machine, then mirror them to the server, but it just confused Inventor
whenever I open a large assembly file, didn't seem to know which file
location to open a file from, local or server. Right now I have 40+ active
project folders (1 per customer) some customers may eventually get multiple
folders depending on future orders. Each customer may have 100-500 parts for
any given order, doesn't include assembly files or drawing files. Most parts
are unique. I'm working with iparts and iassemblies for similar parts and
assemblies. Also trying to get a handle on illogic to drive similar
elements, but I fell I need to resolve this issue before I implement any
automation.



Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[karthur1]

Odd indeed.  I dont think its a bug in inventor causing this problem. If it was something like this in Inventor, we could not use it to get our work done.

Do you use angle constraints orTangent constraints? What type of constraint is failing?  Maybe the geometry moved or was deleted.  If the error that you see is "Relationship was placed with respect to geometry that is no longer available" then that basically means that the feature was deleted after the constraint was placed.

Do you use the same filename on numerous projects?  What I mean is do you have like "layout.ipt", "Master.ipt", etc that you use on all your projects, but they are in different folders?

I usually have to go back and delete unresolved constraints and re-apply them.

You can do it that way, but you dont have to delete them... just edit it and fix the missing part.

If I do a component replace (usually to use a unique part name for a left and right part) I "save copy as" for a left and right part, then do the component replace. The parts are the same geometry as the one replaced, just a different name. Inventor seems to have a problem with this sometimes, then other times it's no problem. Very inconsistent.

Try using the "Save and Replace Component" tool on the productivity panel if you want to create a copy of a part and swap it out in the assembly (I use this tool all the time). A question though, if they are the same geometry, why do you have different parts? I suspect that you actually are mirroring the RH part to get the LH.  If that's the case, you will lose constraints. The geometry is no longer there.

Just curious, what version of Inventor are you using?

Kirk

[blair]

It could be as simple as using the same part in a different IAM and someone has made a small change to that part in another IAM.

If you use Adaptivity and get too many "Adaptive" parts it can blow-up a IAM in quick order. I try and clear Adaptivity as soon as possible when using it in a IAM file. A part then changes a bit and any constraints that referenced that adaptive feature could then fail.

Sketches in IPT files not fully constrained could cause features to fail, any Contraints that rely on these features will blow-up as well.

Since you haven't stated you are getting any "Unresolved Missing Link" we can assume that no parts have been deleted or parts are outside of the Project File.

[Anonymous]

Hi Kirk,

Thanks for the reply. I try not to use angle constraints,
but sometimes it can't be avoided. Tangent is a last resort. The failing
constraints are either mate or flush. Usually. Sometimes the insert goes
wonky too. "Relationship was placed with respect to geometry that is no
longer available" is the most common error, but all the parts and geometry
are still there. As to repairing the constraint, it's usually easier to
delete and reapply because I can't see the offender even though it's
supposed to be highlighted, it's just not. As I mentioned in the original
post, I use sub-assemblies as opposed to one giant assemble, it's just
easier to work that way. (for me) I wish I could upload one of the offending
models, but it's just not practical to do that.

There are common files (and file names) in most of the projects.
(standard parts) kept in a library folder pathed to the different projects.
These parts don't get modified.

As far as left and right (actually Curb side & Road side) These
parts are the same to a point. When I have to modify them I do the CS/RS
swap and make the change. I don't really use mirror in assembly files to
often because the mirrored part is un-constrained. I seem to remember in
Inventor series 11, you could mirror the constraints as well as the part.
Inventor no longer has that option. (wish list)

Thanks for the input and I will definitely try the save and
replace component tool.



Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[Anonymous]

Hi Blair,

Nothing that simple, I am the only user. But I do use
adaptive parts, and have been clearing adaptivity once the part model has
been finalized.

I will have to look at my sketches to make sure they are fully constrained,
they usually are but it won't hurt to check.

Thanks for the input.



Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[karthur1]

Frank,

It would be easiest to see the actual error. It sounds like its something in your workflow.  I'm sure your models are propietery, so it would probably be best to send them to Johnson.

Kirk

[blair]

I see you do Class 8 as well. We primarly specialize in log-transportation trailers/equipment.

[Anonymous]

Kirk,

   save and replace is a great tool! working great when I need to modify a part in place for left and right, and it doesn't lose constraints.

                   Thanks Heaps

                                         Frank

[karthur1]

Frank,

Just curious how are doing your RH / LH parts with the "save and Replace" tool?

Kirk

[Anonymous]

Hey Kirk,

I use a lot of parts from content center (structural
shapes), then once they are in place, I do the save and replace, renaming
for L/R, and then make the modifications for the left and then the right. I
use the assembly model they are placed in to create the cuts needed for left
and right parts. It would be the equivalent of an end treatment, but nothing
like what I need is offered from the frame generator. Sometimes the
modification uses existing geometry to create and sometimes I use the direct
edit tool to create the needed modification. I like the direct edit tool for
tubes and channels as it is much easier than trying to create cutting
geometry to get the desired end.



Frank J. Nagle II

Mechanical Engineer

Summit Trailer Sales Inc.

Summit Station, Pa. 17979

570-754-3511 Ext.17

[edi]

Hi All,
Edi here, A Very Long ~ 20yrs. time user of INVENTOR and Autocad user from v2.?.
I have been chasing the loss of constraints for what seems to be forever.
A resent assembly with 300+ parts exploded on me in front of a customer, I dropped everything to try to understand why.
4 days later, reading a post (1 of hundreds) the author asked, do you have files of the same name in the search path?
I said Hu! Yes I do. As a practice I make backup copies of most large projects (not compressed).
Yesterday I compressed all of the backups and checked for other duplicate files and shut down and reloaded the main assembly. (TaDa!)
Every Constraint was Repaired. This may not Fix your issues but keep in mind the first file inventor finds may be the one it uses.

[edi]

Edi here again,

Well thought I had it, No, I'm still chasing it. This is nuts. So far on this one job it has cost me 2 solid man weeks including weekends. (very expensive) I love inventor but I'm about to ditch Inventor as I have not been able to resolve this issue. I cant afford to continue. I have run into this issue many times on large assembly's at a cost of many thousands of dollars. It's about to cost me this job.

I would welcome suggestions.

[BDCollett]

---

@edi wrote:

Edi here again,

Well thought I had it, No, I'm still chasing it. This is nuts. So far on this one job it has cost me 2 solid man weeks including weekends. (very expensive) I love inventor but I'm about to ditch Inventor as I have not been able to resolve this issue. I cant afford to continue. I have run into this issue many times on large assembly's at a cost of many thousands of dollars. It's about to cost me this job.

I would welcome suggestions.

---

You dug up a 7 yr old thread and have not really given anything to help you with. No files, screenshots etc.

Most of the issues here can be solved by better file management. Use unique filenames, even better use Vault and have that create all the backups and version control. Use a single project file. I have never had these issues.

[karthur1]

---

@BDCollett wrote:

---

---

You dug up a 7 yr old thread and have not really given anything to help you with. No files, screenshots etc.

Most of the issues here can be solved by better file management. Use unique filenames, even better use Vault and have that create all the backups and version control. Use a single project file. I have never had these issues.

---

I agree with this.  If you are having these type issues, it's not Inventor.  The first thing you should look at is to make sure Inventor is loading the correct files in your assembly.

If your using non-unique filenames, you need to have a different .ipj setup for each project. You can still have issues with over-writing files during backups if you are not very careful.