change part coordinate system?

[bobmorey]

Hi I'm sure this has been covered before but I cannot seem to find the answer in help or on this forum.  I'm using INV 2011.  I want to change the part coordinate system from Y axis pointing up to Z pointing up so I can have a part STL printed more effectively.  I tried creating a grounded point, then changing the orientation to Z pointing up but this did not appear to change the overall part orientation.  I have also tried to change the first sketch coordinate system. but this doesn't work either (no geometry visible to define Z direction).  I sketched the part in X-Y plane and extruded it in the -Z direction.  I should have sketched it in X-Z and extruded it in -Y.

I dont think I want a UCS, I want to change the original part orientation in space.

any suggestions would be appreciated.  Thanks, Bob

[scottmoyse]

first of all you should create your own sketch plane before creating a sketch. This will allow you to redefine the plane and all its dependants and maintain more references then if you just redefine the sketch. You could take that theory further and just create your own UCS as a base, which you could then redefine when you need to.

I have seen somewhere you can choose which UCS to use, either the WCS or the user created one, but i can't find it at a glance. Another work around is to export from an assembly since you can't redefine the parts WCS.

[JDMather]

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@scottmoyse wrote:

first of all you should create your own sketch plane before creating a sketch. ....

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I have never done this and don't understand the logic?

There are several ways to change the coordinate system - but we don't bother here.
You can change the part orientation in the RP system software before printing.
Whoever is making the model should be familiar with orienting for best results.
You might find a different service to make your models.

 In 2011 make sure you click Options when saving your stl file and set the correct units.

[scottmoyse]

JD, imagine this. You have a Skeletal Model created using Solid body modelling, its base positioning is governed by its original workplane and reference geometry that has been derived from another source. If you were to reference the sketch to another workplane, then the reference link gets broken. However, if you created a base workplane first and placed the sketch on that, then later on you wanted to redefine the sketch, you just redefine the workplane then the sketch references remain intact, assuming the projections are still within range.

You can create a situation, where you can have a cabinet drawn sitting on the floor, then you could reposition it by sticking on the wall. Obviously you would never want to do that particular example, but its an extreme example to illustrate my point.

Or you can have a square cabinet turned into and angled one, so every angle isn't 90 degrees, (this involves avoiding the horz and vert sketch constraints at all costs!) all by redefining work planes to different angles.

There are several times a week where we need to redefine a sketch so it is starting on a workplane of  a different height, its a very simple and quick change if the sketch wasn't created on any of the parts origin planes. If it was and there were reference geometries involved then there is a lot of sketch rebuilding to do.

[IgorMir]

Hi Scott,

I am with you on this one. I use Muscular modeling technique almost exclusively in my workflow. Once the object is derived into a new part file - first thing I do is creating a Base Plane (I name it that way) which is an offset work plane from the derive component face I want to use.

The only times when I skip on creating the Base Plane is when I can use the default Origin Planes. That's usually for the first component in the design or for standard off the shelf items. But then again, if changing the direction of Z-axis is anticipated (Flip Normal) - the creation of zero offset work plane first (Base Plane)  is a good idea.

Regards,

Igor. 

[scottmoyse]

I'm glad someone else sees the point, and makes use of it.

[Anonymous]

Three simple steps:

1. Determine which plane you want the base of your part/assembly to lie on

2. If this plane is one of the 3 standard planes (YZ, XZ, XY) right click it in the browser and turn on visibility. (If not then create your own plane)

3. Constrain a face parallel to the base of your part with this plane using a standard mate constraint.

I hope this answered your question.

Best of luck,

Edward Doyle

[alihillaldam]

JD, Mate, based on Cartesian coordinate system, in engineering, math, geometry and physics, at least from what I studied from primary school until now "Z" is always pointing up not side. http://en.wikipedia.org/wiki/Cartesian_coordinate_system http://en.wikipedia.org/wiki/Right-hand_rule You may not need it but some people like me need to know how to change it.

[Anonymous]

Here is what i did to change my life in inventor to the right handed coordinate system. (Z pointing upwards)

Basicly, you define a UCS and save as a new template, and use it all the time.

1- create new part. Select standard.ipt template (or what ever you're using), click finish sketch.

2- align the view to the front. (click on the front face of the navigation cube on the top right, rotate the view..etc)

3- From models ribbon, select UCS. Expand the 'origin' on the left panel 'model browser' to select center point, as UCS origin.

4- Now that you defined the coordinate system right handed, you can as well select the XY plane as 'TOP'. You can do this by, again aligning the view to front, then selecing 'Set this view as>Top' from the context menu of the navigation cube on the top right, 

5- Save Copy as Template from the Save As... menu. Give it a name. Close this file

6- Create new part and use this new template instead of Standard.ipt rest of your days.

[JDMather]

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@alihillaldam wrote:

... "Z" is always pointing up not side.

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What is "up"?  What is "side"?

In all the programs that I use and in all the mathematics classes I have had the relationship between x, y and z is an agreed upon convention.

From your link

"When choosing three vectors that must be at right angles to each other, there are two distinct solutions, so when expressing this idea in mathematics, one must remove the ambiguity of which solution is meant.

There are variations on the mnemonic depending on context, but all variations are related to the one idea of choosing a convention."

Oops, I got this old thread confused with this more recent thread

http://forums.autodesk.com/t5/Autodesk-Inventor/best-way-to-set-up-drawing/td-p/4481237

If you have a reason to set up a coordinate system relative to the base coordinate system, do so.  But that doesn't change convention between x,y and z.  Makes use of the standard convention.

[barttexx]

thank you, help me 😄 simple think, but brain not working any more 😄

[wschleter]

This is the one that worked for me. My interpretation of the original question was "how do you change the coordinate system used by STL output". Inventor seems to use the 'world' coordinate system no matter what the current sketch plane/UCS is. Creating a new assembly with the part oriented like you want it printed worked because then inventor uses the coordinate system of the assembly as the STL output coordinate system.

[dswilson22]

Automotive CAD programs Catia, NX, Rhino and yes even Autodesk's Alias use Z up.

There should be an option in the Inventor aplication settings to simply choose Z or Y up. Those are the two conventions.

Maya has the option.

Fusion 360 gets this mucked up within itself unless they've fixed it.

A user shouldn't have to create a new part and/or assembly file, modify its origin orientation (apparently not its UCS or sketching plane systems), and save a unique template to be used.

If Inventor want to be taken seriously by automotive folks, it should make it easy for them to adapt.

There should be a result in the help system if it is searched for "Z up".

I think I have it figured out, again, as I have newly installed Inventor 2016.

There just should be an option in the Inventor aplication settings to set Z up.

[MwakiM]

I think these two posts from a while ago are simple and enlightening:

https://archive.org/details/bliptv-20131014-195528-Caseinc-InventorMakingZYourUpAxisRatherThanY228

http://cadsetterout.com/inventor-tutorials/start-your-sketch-right/

[rmahendra]

If you want to change your document or Templates orientation to the vehicle coordinate system, that is the Z axis facing the top direction, go to the Tools>Document Settings>Modeling>User Coordinate System Settings. If it works, give it a Thumbs Up..

[lmc.engineering]

Call me stupid, or maybe it doesn't exist in Inv2011, but under modify tab there is the Move bodies command. You can rotate things from there.. It's not my first choice of action if I ever need to change a UCS, but it'll work for your dilemma.

All the best

[rmahendra]

@lmc.engineeringBut, The same options are available in the Lates versions too, it's called Flexible, So you can rotate a solid body ( u can rotate one body at a time and if you have a multi-body part, then you are going to rotate every body manually), to different coordinates. But that you have to do for every part that is in a wrong coordinate system, but the option I showed is a one time setting that will make all the parts you create default z towards the up.

Thanks

Mahendra Nathan

[lmc.engineering]

I'd never dream of rotating multiple solid bodies like this.. it was just another suggestion for a simple fix. If a single solid is 90degrees out, I'll probably just rotate it. Job done.

[dpeters2]

I would insert your part into a new, blank assembly file, and constrain it so that the assembly file's world z-axis is pointing the way you need it to relative to your part.  Then derive that assembly into a new part.  Now you'll have a part with the world UCS just the way you want it.

Doing it this way, the UCS is in the derived part can also be changed - by re-constraining the original part in the intermediate assembly file.

[steven_devries]

I am really curious what the "Modeling > User Coordinate System > Default Plane" actually does. 

In Inventor 2024, it seems to do nothing at all.

When I click 2D sketch button it still turns to face the XY plane and not XZ plane. 

Even after saving / closing and re-opening the file.

It also does not change the cube orientation to Z up.

Maybe it used to work and is now broken?