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Inventor Sketch Orientation

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Message 1 of 52
mikeg
7551 Views, 51 Replies

Inventor Sketch Orientation

This is something that annoys me to no end and that I have never seen explained . Why the heck does Inventor arbitrarily orient sketches as it sees fit? I often create my first sketch on the right (YZ) plane and Inventor, stupidly turns the sketch where "RIGHT" in the view cube reads from top to bottom. This is totally absurd.

I know all the things to do to AFTER this happens, but it shouldn't happen in the first place. If I turn my sketch so that up is up, like it should be, I then have to remember that vertical is horizontal, which is now vertical. I can't change the sketch coordinate system. It's the first sketch and there is nothing to align it to.

Autodesk has to have an explanation for this, but I haven't heard it. Maybe someone would be so kind as to fill me in and, if possible, how to prevent the above example from occurring in the first place.

This, and the fact that I can't dimension to any existing vertices or edges without projecting them first, really make me hate using Inventor sometimes. To me, these are huge problems, neither of which Solidworks has. At worst, both of these behaviors should be configurable.

Thanks
Mike
51 REPLIES 51
Message 41 of 52
swhite
in reply to: mikeg

But sketching on the x,y axis with Z towards you IS the proper way. only if you look at a plane from the top is z pointing upwards. The z coordinate is always towards you, not specifically up. The only time the z coordinate points upwards is if you look at a model from a perspective view, then z is up simply for convention sake. But we are drafters and modelers, all coordinates are always given on the x, y coordinate regardless if it is Front, Top or Side view, with z strictly for the modeling side. A hangover from the days when there were no 3D modeling programs, only the x,y, coordinate mattered on your drawing.

Axis1.jpg

Another benefit is all FG parts are placed on the drawing by default in what you would consider thier default front view, regardless of thier model orientation. Since our company uses FG almost exclusively, to us this is a good thing.

Steven White
Lee C. Moore, Inc.
www.lcm-wci.com
Inventor 2011
Intel Dual Xeon E31225 @ 3.1 GHz CPU
16 GB RAM
NVIDIA Quadro 600 GPU
Windows 7 - 64 Bit
Message 42 of 52
ihiengdept
in reply to: swhite

I didn't really mean to set off a debate about what is the proper plane to sketch in or the proper axis for the direction of gravity.  It's somewhat of a tangent to the discussion.  There are bound to be multiple opinions and no right answer for that.  (I tend to think about this issue in terms of "horizontal plane" which will always be the plane perpendicular to your gravitaional axis).  Once you choose which way is up, using a RH coordinate system, the rest of the decisions fall like dominos.  

 

It could be as graemev indicates, where Z is your vertical.  (This is how our CNC is programmed).  Or as swhite suggests with XY being your sketch plane, with Y as vertical and Z is "depth".  This makes a lot of sense for some parts we work with.  (We build machines that work with extruded material and this makes a lot of sense in many cases.)  This can be debated adnauseum and beyond my synopsis here, I don't care what Audoesk chooses if I have the option to change it.  (The merits of both have actually already been brought up in the thread before I even joined.)

 

At best Autodesk can only flip a coin, pick it's poison and move on.  I was wondering if they provided an option to select this, and although I haven't seen a "horizontal plane" option, now that I think of it, there is a "direction of gravity" option that I've seen somewhere.  I'll check on that.

 

The mistake Autodesk made was that their cube which says "top" is not consistent with the gravitational axis in their default template.  It is a mistake that caises flukey 90 deg rotations for people.  It should be fixed.  I'm not critiquing a choice of A over B.  But the inconsistency of using method A in one part, and method B in the other.

 

I really don't care whether they change the cube or the gravitational axis because 1/2 the people will think it was the right one, and the other 1/2 won't.  Right now they've found a way to confuse 95% of new users using the default template (in imperial units, if that makes a difference).  

Message 43 of 52
prem
in reply to: mikeg

The change in the orientation is in respect to ISO and DIN Standards of Project (Metric Part Templates ), The ISO uses the First Angle of Project hence the view reverses, While the DIN Uses the Third Angle of Project. This may suprise but yes it also effects the Part templates and not only Drawing templates

 

This may be to late in the discussion forum, Hope it Helps!!

Thanks
Prem
Windows 7 64 Bit
16 Gigs of RAM
Intel I7
Nvdia Quadro 3000M
Message 44 of 52
ihiengdept
in reply to: prem

That's good information. It doesn't really solve the problem, but it explains a little more about the cause.

Unfortunately, the frustration continues with this. I've done what I can to make my templates consistent, but I've still seen a few odd behaviors here and there & files created with older templates (the Autodesk default templates) still have the inconsistencies.

I can't help but feel the core of the issue is that Autodesk gives me a template that is supposed to be "english", but only made half the changes that they should in the template. It's been a while since I dug in to analyze the source of the problem, but in essence, I believe the internal "gravity" direction was not agreeing with the view cube. This breaks the "Look at sketch plane on sketch creation" option (causes the rotations to be wild), and it makes adding "horizontal" or "vertical" constraints unpredictable (something I've learned to avoid, although they can be very convenient for aligning features.)

I don't know if the metric template has these issues. I might have to try that.
Message 45 of 52
ihiengdept
in reply to: ihiengdept

I checked the other templates, they all have the issues except the metric (DIN) one.

Here's a good synopsis of the problem.

Default Template Problems Chart

 

Message 46 of 52
prem
in reply to: swhite

Yes, it should as it uses the 3rd Angle of Projection, so i guess mystery solved, but i have to figure out how to set the Angle of projectinos for Part templates then.

Thanks
Prem
Windows 7 64 Bit
16 Gigs of RAM
Intel I7
Nvdia Quadro 3000M
Message 47 of 52
ihiengdept
in reply to: prem

I should probably start by clarifying that each screenshot above was taken with "Look at sketch plane on sketch creation" turned on, so each screenshot was taken as Autodesk "auto-rotates" to orient the view.

 

On further thought, I don't see how orthographic projection could be related to this issue since it only has to do with a 3D to 2D projection and all views are 3D. The only change shown by the above screenshots between "Standard" & "DIN" is the view cube orientation. In all three cases it auto-rotates to the exact same right-handed, XYZ orientation ignoring what the view cube is set up to be. The DIN standard may specify "Z" as the vertical axis(guessing on this), which orients the view cube correctly and fixes the problem, but I haven't found any information suggesting 1st or 3rd angle defines Z as "up".  

 

You can change the view cube orientation, but the internal mechanics of "vertical" are always the same. I need a way to change vertical in a part template, or else "Z" is always "up" and we are forced to reorienting the cube (which is the only work-around I know).

Message 48 of 52
JSimeroth
in reply to: mikeg

Mike,

I'm right there with you. I found your thread by googling something like " why in the WORLD does inventor flip its orientation all over the place if I decide to start a sketch on anything but the xy plane?!" It literally doesn't make ANY sense to turn 180 degrees to sketch on the xz plane. why. why? WHY?

 

No solution here. Just thought I would tell you you're not alone.

Best of luck. PLEASE let me know if you find a solution.

 

Johnathan

Message 49 of 52

3 years after this discussion was started, and still no resolution.

 

It blows my mind how many people here didn't grasp the real issue. Oh, and that Autodesk never chimed in.


Sketch orientation can be worked around or glossed over when drawing lines or curves because ultimately the geometry will still look correct in 3d.

 

However I have an example which makes it clear. I want to emboss text onto an existing feature. This has nothing to do with first sketch orientation, blah, blah, blah. Inventor automatically selects the x,y,z coordinates when I select my sketch plane. I can "edit coordinate system" but it only lets me edit x and y. It will not let me flip the z direction. Because of this, the text I want to emboss is sideways and reads in reverse.

 

Below image is the sketch mode view:

inventors xyz selection.JPG

 

Below image shows the result in 3D. In this view, I need the text to read correctly. (note current x and y position of the sketch)

sideward text.JPG

 

Below, I used "edit sketch coordinates" to change the x an y. Still, the text is not correct.

edited xy coordinate.JPG

Inventor lets me reorient x and y, but gives no control over the direction of x or y. At this point, I need to be able to flip the x direction and hold the y direction, so that the text reads correctly. But so far, no luck.

 

Another thought would be to flip the "z" direction of the sketch (or draw on the other side of the plane), but I cannot see how to do that either.

 

I worked in Pro-E for 15 years, and now 2 years in Inventor. In Pro-E you could easily define your x,y,z for each sketch. This was no issue.

 

I believe this illustrates the problem the original poster was talking about. This in not a settings or template problem. We need control of the coordinates in the sketch.

 

Using Inventor Pro 2014

Tags (2)
Message 50 of 52

The solution to the emboss issue is solved by constraining the text box.
Not perfect but not unreasonable...
Flow state:
Maximum challenge with maximum skills.
Message 51 of 52

Right after I got done ranting, I found my solution:

 

On the work plane that you are sketching on, you can "flip normal"

FLIP PLANE.JPG

 

Now, my x,y,z are all correct.

CORRECT.JPG

 

So, it looks like a combination of "flip normal" on the plane and "edit sketch coordinates" on the sketch will get the job done. A bit cumbersome, but it works.

Message 52 of 52

@keith.stephensVDUW8

Right click on your work plane and select Flip Normal.  The sketch's postive Z is in the direction of the plane's normal.  Origin planes can't be flipped, of course, nor can model faces-- they're fixed.  If you need a plane facing the other direction at the location of one of the origin planes or part faces, then do a zero offset plane and flip normal.

 

Edit: I see you found it...

 

Hope that helps,

Sam B

Inventor Professional 2016 R3 SP2
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1
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