Invalid Axis/ origin

[G.Hunter]

I have a number of steel door models generated that are controlled by ilogic, see example frame part attached with some errors.

There are a number of errors that seem to arise when some combination of features are enabled, or some sizes are modified. The errors typically do not show until some combination is reached, and we have too many options to test every outcome. For example some axis / origin errors occur on some features when a profile is extruded past say 3 metres (no idea why). The attached frame part was working fine, then extruded to 3200 where some errors arose. The axis were redefined, and the part was extruded back to 2100. More axis errors that were not there in the first place! (as seen attached)

Can anyone explain why this is happening? I am guessing that some features are modifying the plane/face that a feature is sketched on and causes it to lose the origin / axis?

As a fix I am redefining the origin of the feature to the "Centre Point" of the model and using the origin axis (z in most cases) for the y value. Can anyone confirm if this will cause issues, as I believe the previous origin was a corner of the sheet metal face where a feature was modelled? My thoughts are to redefine any errors to the centre point of the model as it should not change, but why does inventor not use this in the first place? Is there a setting somewhere to enable this?

I appreciate this will not be seen as an issue by many, but the nature of our production means creating thousands of copy models off one set of library models, so small issues like this can turn into big problems when features fail.

We are using inventor 2013 SP2 but this has been a problem for many years now, and seems to be getting worse.

[johnsonshiue]

Hi! When work plane or axis fails to compute, ususally it means the source geometry defining the work plane or axis is missing or Inventor has trouble defining the work plane or axis. I took a look at the part but I could not figure out where the failure is. Could you show me the steps resulting in work plane or axis failing to compute?

Thanks!

[mrattray · Accepted solution]

I also see this problem regularly, and have not found a solid cure. It doesn't even have anything to do with how you sketch, the problem is entirely related to the way that Inventor defines its sketches.

There are a few ideas in the idea station for this, but they don't have much love. Go vote for them to help steer AutoDesk's attention towards this problem. Here's a link to one of them:
http://forums.autodesk.com/t5/Inventor-IdeaStation/Sketch-Coordinate-System/idi-p/3720738

[JDMather · Accepted solution]

I did not take a lot of time to look at this, but I would suggest making far less use of projected part geometry.  I didn't see much if any need to project part edges (other than for maybe the Mitre - and not sure really needed there).

I would only project origin planes, axes and centerpoint if possible.

Put all sketches possible on origin planes rather than part faces.  It looks to me like all sketches could have been placed on origin planes.

Use Origin Axis to define Rectangular Pattern directions rather than part edges.

I don't know if these tips would have helped in this case, but I would particularly avoid projections fron the Mitre edges.

I follow these tips and never see this issue.

My opinion for parts that I want really robust under change - I should be able to delete every feature (after finishing the part completely) and still have all the information (in part sketches on origin planes) to rebuild the features without any errors.

The geometry is going to change - that is the purpose if the iPart. But my sketches (other than size) are not going to change.

[G.Hunter]

I am in agreement regarding origin planes being more robust, but it could be a painful process to redraw all our models and redefine all features. If we decide to rebuild in future I believe we will follow this path.

In the mean time I will redefine origins where errors occur under testing. I would be interested if inventor could be set up to use the centre point and origin axis as sketch origins by default.

[JDMather]

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@G.Hunter wrote:
... I would be interested if inventor could be set up to use the centre point and origin axis as sketch origins by default.

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I thought it did?  Tools>Application Options.....
Developing robust modeling techniques is an on-going process.
I look at stuff I did last year, or last month, or last week, or yesterday..... .... and shudder.

But try to improve technique on all future work.

The more something is likey to change (like iParts) the more time I spend trying to get everything referenced to the origin (BORN Technique) rather than using a part face/edge for reference.

[G.Hunter]

We currently have "Autoproject edges for sketch creation and edit" unchecked, and we have "Autoproject part origin on sketch create" checked.

I think there was a time when we had the first one checked, is this what is causing the errors? Or am I missing something here?

[JDMather]

I never use Autoproject edges.

I can't believe that Autodesk sets this as the default install.  Really shakes my confidence in them.

[mrattray]

JD: I think there may be some terminology confusion in this thread between the sketch origin/axis and the projected model origin.
G. Hunter: there is no options controlling this behaviour available to you currently.

[swalton]

The Invalid Axis/Origin error is related to the local coordinate system Inventor automatically creates when the user starts a sketch. 

When the user creates a sketch on a feature face, Inventor grabs an edge and endpoint to define the horizontal and vertical axis for the sketch.  It does not use the origin folder workfeatures.  I think, but have not tested, that if the user creates sketches on the origin planes, Inventor will use the origin folder workfeatures to define the local sketch coordinate system.

The error is triggered when the user makes a change to the base geometry that alters/eliminates the endpoint/edge used for the sketch. 

I don't see this error often, but I do see it. 

Ways to avoid it:

1. Sketch on origin work planes not on feature faces.  This might also work if you create workplanes for sketches rather than use feature faces.  Experiments may be in order.

2. Build your features in an order that does not destroy edges/endpoints that are critical to downstream sketches.  This takes experience and/or redfining the sketch after it is created.  Autodesk could make this simpler by adding the option to define the local coordinate system as part of sketch creation (similar to how PTC/Creo works).

[JDMather]

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@mrattray wrote:
JD: I think there may be some terminology confusion in this thread between the sketch origin/axis and the projected model origin.

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Someone posted a really good (and scary) example here a few months ago.  I thought I saved it, but now can't find the file or reproduce a worrisom example.  I'll do a bit more searching.

 I found it - Post #8.  http://forums.autodesk.com/t5/Inventor-General/Axes-rotated-in-a-part-file/m-p/4415823#M482202

Let me get this documented.

[hmXB94V]

That totally cracked the nut for me. Redefine the sketch and hereby re-choosing the plane to draw on and then the projected geometry also cooperated. this hint solved everything for me.

[karthur1]

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@G.Hunter wrote:
...

As a fix I am redefining the origin of the feature to the "Centre Point" of the model and using the origin axis (z in most cases) for the y value. Can anyone confirm if this will cause issues, as I believe the previous origin was a corner of the sheet metal face where a feature was modelled? My thoughts are to redefine any errors to the centre point of the model as it should not change, but why does inventor not use this in the first place? Is there a setting somewhere to enable this?

I appreciate this will not be seen as an issue by many, but the nature of our production means creating thousands of copy models off one set of library models, so small issues like this can turn into big problems when features fail.

We are using inventor 2013 SP2 but this has been a problem for many years now, and seems to be getting worse.

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My thoughts exactly.  I put up a Ideastation post to try get get something done on this.  It would be great if Inventor would use the origin center rather than an edge of a part.

Vote for the idea if you think it applies here.

Thanks,

Kirk