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invalid axis/origin

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Message 1 of 22
cadman777
1520 Views, 21 Replies

invalid axis/origin

this question arises out of a persistent problem that i've encountered over the years of using inventor.
i'm trying to prevent 'redefining' the sketch in order to get it to not be broken after a part change.
has anybody had this problem and found and quick a simple solution to it?
here's what happens:
1. a plate part is created with all the cutouts on it;
2. a new part is created with said plate as a derived component inside of it;
3. a sketch is created that uses the derived component's features as outlines to define cut areas;
4. the desired area is cut away and the remainder constitutes the desired part;
5. other parts are created this same way, only the rest of the plate is parted-out such that each part, when constrained together with all the othe derived parts in the configuration of the original part, comprise the original part, yet in pieces, like a puzzle.
6. the original plate areas get modified after the fact, due to change orders by the customer;
7. the derived parts all end up with the cutting sketch (only one cutting sketch per file) broken;
8. the error from the Sketch Doctor is this, "invalid axis/origin"
9. although I open the cutting sketch and re-assign the axis/origin to another point on the part, the broken sketch never gets fixed, no matter where I re-assign the origin on the part.
CAN I reattach the origin like that? If not, then how can I do this so that I don't have to REDEFINE the sketch on the original surface of the derived part?
I have ALWAYS had to REDEFINE the sketch in order to fix the broken axis/origin.
When that is done, the ENTIRE DOWN-STREAM set of features gets BROKEN.
The result is a TIME-CONSUMING repair on the part.
Does anybody have a quick and easy way to fix this "invalid axis/origin" problem on sketches in derived parts?
... Chris Edited by: cadman777 on Jul 30, 2009 9:18 AM
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
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21 REPLIES 21
Message 2 of 22
Anonymous
in reply to: cadman777

It sounds like your building a progressive die is that true?

Tim
Message 3 of 22
cadman777
in reply to: cadman777

Tim,
It's a deck plate for a mining sled.
I do this frequently when there's a planar surface that is cut up into various pieces.
It's an easy way to do in-context modeling, and keep everything updating to the top level model during the design process.
Any ideas how I can fix these nasty, time consuming lost origins in my sketches?
... Chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
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Message 4 of 22
JDMather
in reply to: cadman777

Are you creating sketches on part faces or on Origin workplanes?

I always use the origin workplanes as much as practical and only Project Geometry the geometry that is absolutely necessary. I never see this error in my work but do see it in my students work.

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Message 5 of 22
Anonymous
in reply to: cadman777

I agree with JDMather that this is related to how the sketch is located. It
appears that you are creating the sketch on a face in the derived part, then
editing the master and removing material which eliminates that face (or at
least the part of the face that the sketch origin is attached to). Using the
Origin planes for sketches in the derived part should help. Also as JD
mentioned, you'll have to give some forethought to which geometry you
project for the same reason. You cannot anticipate every change, but you
probably have a good idea of what is typical for your designs.


--
Patrick Miller
Autodesk Manufacturing Industry Group
Technical Publications - Subject Matter Expert
Novi, MI
wrote in message news:6228101@discussion.autodesk.com...
Are you creating sketches on part faces or on Origin workplanes?

I always use the origin workplanes as much as practical and only Project
Geometry the geometry that is absolutely necessary. I never see this error
in my work but do see it in my students work.
Message 6 of 22
cadman777
in reply to: cadman777

JD/Patrick,
Thanks for the tip.
I'll try to do it that way from now on, and see if it performs better.
I just wish I knew how the software processes these kinds of entities, so I can use it better with less problems.
Cheers ... Chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
Message 7 of 22
Anonymous
in reply to: cadman777

As others have have already said, this is most likely because some of the
derived geometry (edges and vertices) used for the sketch geometry
disappeared after the edits you made. One thing you can do is to define an
empty sketch in the base part and then derive that sketch to your derived
part. You could add the necessary sketch geometry to this sketch within the
derived part. A sketch defined in the base part is far more stable than one
defined in the derived part.

wrote in message news:6227927@discussion.autodesk.com...
this question arises out of a persistent problem that i've encountered over
the years of using inventor.
i'm trying to prevent 'redefining' the sketch in order to get it to not be
broken after a part change.
has anybody had this problem and found and quick a simple solution to it?
here's what happens:
1. a plate part is created with all the cutouts on it;
2. a new part is created with said plate as a derived component inside of
it;
3. a sketch is created that uses the derived component's features as
outlines to define cut areas;
4. the desired area is cut away and the remainder constitutes the desired
part;
5. other parts are created this same way, only the rest of the plate is
parted-out such that each part, when constrained together with all the othe
derived parts in the configuration of the original part, comprise the
original part, yet in pieces, like a puzzle.
6. the original plate areas get modified after the fact, due to change
orders by the customer;
7. the derived parts all end up with the cutting sketch (only one cutting
sketch per file) broken;
8. the error from the Sketch Doctor is this, "invalid axis/origin"
9. although I open the cutting sketch and re-assign the axis/origin to
another point on the part, the broken sketch never gets fixed, no matter
where I re-assign the origin on the part.
CAN I reattach the origin like that? If not, then how can I do this so that
I don't have to REDEFINE the sketch on the original surface of the derived
part?
I have ALWAYS had to REDEFINE the sketch in order to fix the broken
axis/origin.
When that is done, the ENTIRE DOWN-STREAM set of features gets BROKEN.
The result is a TIME-CONSUMING repair on the part.
Does anybody have a quick and easy way to fix this "invalid axis/origin"
problem on sketches in derived parts?
... Chris

Edited by: cadman777 on Jul 30, 2009 9:18 AM
Message 8 of 22
Anonymous
in reply to: cadman777

You could avoid this situation by defining an empty sketch in the base part
and deriving it. You would then add the desired sketch geomtry into this
derived sketch. A sketch defined in the base part is far more stable than
one defined in the derived part.


wrote in message news:6227927@discussion.autodesk.com...
this question arises out of a persistent problem that i've encountered over
the years of using inventor.
i'm trying to prevent 'redefining' the sketch in order to get it to not be
broken after a part change.
has anybody had this problem and found and quick a simple solution to it?
here's what happens:
1. a plate part is created with all the cutouts on it;
2. a new part is created with said plate as a derived component inside of
it;
3. a sketch is created that uses the derived component's features as
outlines to define cut areas;
4. the desired area is cut away and the remainder constitutes the desired
part;
5. other parts are created this same way, only the rest of the plate is
parted-out such that each part, when constrained together with all the othe
derived parts in the configuration of the original part, comprise the
original part, yet in pieces, like a puzzle.
6. the original plate areas get modified after the fact, due to change
orders by the customer;
7. the derived parts all end up with the cutting sketch (only one cutting
sketch per file) broken;
8. the error from the Sketch Doctor is this, "invalid axis/origin"
9. although I open the cutting sketch and re-assign the axis/origin to
another point on the part, the broken sketch never gets fixed, no matter
where I re-assign the origin on the part.
CAN I reattach the origin like that? If not, then how can I do this so that
I don't have to REDEFINE the sketch on the original surface of the derived
part?
I have ALWAYS had to REDEFINE the sketch in order to fix the broken
axis/origin.
When that is done, the ENTIRE DOWN-STREAM set of features gets BROKEN.
The result is a TIME-CONSUMING repair on the part.
Does anybody have a quick and easy way to fix this "invalid axis/origin"
problem on sketches in derived parts?
... Chris

Edited by: cadman777 on Jul 30, 2009 9:18 AM
Message 9 of 22
cadman777
in reply to: cadman777

do you mean:
1. i should make the entire plate profile (as split up into it's various pieces), in a sketch that exists in an empty part;
2. then use that part-sketch as a derived component in another part, in order to make from it one of the plate parts;
3. then repeat this process for every part of the overall plate?
if so, is this more stable then doing what the other suggestion was?
I've done this before, and it seems to be ok until i change the original sketch.
sometimes it works, and sometimes it doesn't.
the big questions are this:
WHAT PARADIGM DOES INVENTOR ANCHOR THE SKETCH TO THE ORIGIN?
WHERE DOES INVENTOR ANCHOR THE SKETCH TO THE ORIGIN?
... chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
Message 10 of 22
swalton
in reply to: cadman777

Have you turned off auto project edges in your application options?

If you do this, IV won't project any edges at sketch creation. You then have to project the edges that you need to define the sketch. The fewer edges projected in your sketch, the fewer things to break. You might want to turn on the auto-project part origin to give you a constant point in the sketch.

It would be nice if IV would project perpendicular faces as a construction line so sketches were not dependant on edges. faces seem to be more stable than edges.

It would be nice if IV had a tool to re-link projected geometry. If a project edge is lost, I want to be able to right-click on the broken projected geometry, select the re-link command and then select a new edge to drive the projected geometry. I know about break link, but I want heal link.

Steve Walton
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Message 11 of 22
Anonymous
in reply to: cadman777

I think I didn't explain properly.Replacing the step 3 in your work flow, by
a few more steps...

1. a plate part is created with all the cutouts on it;
2. a new part is created with said plate as a derived component inside of
it;
3a. create an empty sketch in the plate part (I assume that you can identify
the face corresponding to the one on the derived part where you want to
create the sketch exist on the plate part)
3b. derive this sketch into the derived part (by editing the derived part).
3c. complete this sketch by defining cut areas (most probably you would need
to project edges or faces).
4. the desired area is cut away and the remainder constitutes the desired
part;

Instead of creating an empty sketch in the plate part you could have created
a work plane there, derived the work plane and created a sketch on that
derived work plane. This should be similarly more stable. The important
thing is to define the coodinate system of the sketch in the plate part.

As to your question on how a sketch is "anchored", when you create a sketch
based on a face, often we try to pick an edge, based on many criteria, as
one of the axes. As a user I don't think it's particularly helpful to
understand that algorithm. If you try to redefine the sketch coordinate
system you could, in most cases, figure out how the sketch is "anchored."
You could, of course, use this command to redefine the sketch, before you
start sketching.

I hope I answered your questions.

wrote in message news:6228425@discussion.autodesk.com...
do you mean:
1. i should make the entire plate profile (as split up into it's various
pieces), in a sketch that exists in an empty part;
2. then use that part-sketch as a derived component in another part, in
order to make from it one of the plate parts;
3. then repeat this process for every part of the overall plate?
if so, is this more stable then doing what the other suggestion was?
I've done this before, and it seems to be ok until i change the original
sketch.
sometimes it works, and sometimes it doesn't.
the big questions are this:
WHAT PARADIGM DOES INVENTOR ANCHOR THE SKETCH TO THE ORIGIN?
WHERE DOES INVENTOR ANCHOR THE SKETCH TO THE ORIGIN?
... chris
Message 12 of 22
cadman777
in reply to: cadman777

i have 'auto project' ON
guess i'll have to turn it off
what's the purpose of having 'auto project' if it doesn't work right?
if it's broke to begin with, why not OMIT IT FROM FUTURE RELEASES?
i nearly never use 'adaptive parts' b/c they ALWAYS break in iam files (like cable, lines &tc), whereas a the cable module is way too much overhead for just a few cables.
i already have project origin.
i was one of those who 'whined' about it until it majically appeared in a future release so long ago.
i agree with adsk fixing the usability issues in down-stream sketches.

this is what i get from the discussion thus far:
i have 2 options here:
1. turn off autoproject and sketch in a derived part on the fixed origin plane, OR
2. turn off autoproject and use an empty part-sketch as a derived component to create a 3d solid part.
which option is the most stable?
... chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
Message 13 of 22
cadman777
in reply to: cadman777

thanks for your input
what you mean is clearer now
however, it got much more complicated
the software should be programmed so that accomplishing this should be simple and easy
the more levels deep a part goes, the more prone to error it is on a change, OR the more the system boggs down
i recently designed a piece of mining equipment that had a sheet metal cabin
i tried 8 different ways to connect all the sheet metal wall plates to a base sketch, in order to prevent errors in final size and fit of all parts
it's amazing how many levels deep some of the plates got, due to dependencies on how the cabin was fabricated
the caveat was the enormous amount of overhead in the model on the computer
however, i believe what i did was a trade-off:
i traded speed for reduction of error prone model parts
i always try to err on the side of caution, b/c @ 9 tons of 12 ga stainless steel (x 3, b/c we made 3 of these), the cost from errors could have been extremely high
however, we had minimal errors, and minimal consequent cost (less than 1% on the overall project)
was that due to inventor?
only partly
mostly it was due to how i chose to use the tool
i could have done it better in SW, had i known how to use that program back then (b/c of how good their sheet metal module is)
in any case, thanks for your help
i will test-out a few options based on what's been written in here, since nobody has been able to tell me conclusively what method is the most stable
... chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
Message 14 of 22
scottmoyse
in reply to: cadman777

If you project an entire face after the sketch is created. Then when the link is broken you can edit the sketch and RMB on the entity and it gives you the option to redefine, this includes a new face.

Scott Moyse
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Message 15 of 22
cadman777
in reply to: cadman777

scott,
that's what i've been forced to, but want to avoid
the reason i want to avoid this is b/c the creation of a new feature screws up all the down-stream features that are dependent upon the new feature
... chris
... Chris
Win 7 Pro 64 bit + IV 2010 Suite
ASUS X79 Deluxe
Intel i7 3820 4.4 O/C
64 Gig ADATA RAM
Nvidia Quadro M5000 8 Gig
3d Connexion Space Navigator
Message 16 of 22
NeilClasby75
in reply to: cadman777

I have just had the 'invalid axis/origin' error on an old part. I have, since then, changed the way I draw working with workplanes much more. But I don't understand why this error is occuring as the feature created from the sketch (which is not shared) is suppressed as the part is an iPart. When I change to the member that computes the feature it is fine; I only get the problem when I switch to a member that suppresses the feature, but then get the error even though the sketch is not being used! How annoying! If the supression worked on the sketch as well as the feature then I would not get the error.

I can probably suppress the dimesions of this sketch separately, but that seems over the top.

Cheers, Neil.
Message 17 of 22
wim001
in reply to: cadman777

Indeed, working with the planes in the derived part and the sketch on the origin plane is more stable.
Message 18 of 22
dan_inv09
in reply to: cadman777

Does it stop the part from working?
(Or is the problem just OCD? :))
Message 19 of 22
NeilClasby75
in reply to: cadman777

Hi Dan

Not sure what OCD stands for?

But no it doesn't stop the part working, it just makes the info symbol in the browser and the doctor highlighted. Annoying as I like parts to be perfect. I had to do a scheduler update with total rebuild and it did so without error.
Message 20 of 22
dan_inv09
in reply to: cadman777

I like things to be perfect as well, but we have to learn that sometimes things are "good enough."

"Obsessive Compulsive Disorder"

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