Inventor Sketch Orientation

[mikeg]

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

[Anonymous]

They are.

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[JDMather]

>...and the fact that I can't dimension to any existing ...edges without projecting them first...

Works fine in Inventor here.

JD
Certified SolidWorks Professional
Inventor 2009 Certified Professional

[Anonymous]

Whenever you're in sketch-mode just remember the
thicker grid-line running through the origin is "horizontal" 

Better yet - change the sketch options from
horizontal & vertical to parallel & perpendicular - then only ever need
to have 1 line with a horizontal or vertical constraint.

yes, I know it's confusing at times, but surely far
easier (especially for people new to 3d-cad) than the mess of MDT with
reassigning the coordinate system depending on where you're sketching (not
that I could remember how to use MDT these days, but do remember changing
coordinates at times).

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<mikeg@goughecon.com>
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href="news:6125408@discussion.autodesk.com">news:6125408@discussion.autodesk.com...

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

[Anonymous]

Tools  > Application Options
> Sketch

Also look into App Options >> Display View Cube
settings

Possibly a different template with defaults set to
YZ.

--
Dennis Jeffrey, Autodesk Inventor Certified
Expert
Autodesk Manufacturing Implementation Certified
Expert.
Instructor/Author/Sr. App Engr.
AIP 2008 SP2, AIP 2009-SP1
PcCillin AV
HP zv5000  AMD64 2GB - Geforce Go 440, Driver: .8185
XP
Pro SP3, Windows XP Silver Theme

href="http://teknigroup.com">http://teknigroup.com

[mikeg]

Dennis,

There is nothing in Sketch options to control the sketch orientation. I've tried everything, over the last several versions, and it's still the same way.

Also, the problem isn't the orientation of the view cube. I can reset it to whatever I want. But that doesn't stop Inventor from rotating the orientation of sketches created on the YZ plane 90 degrees CW and those created on the YZ plane 180 degrees.

I would love to here Autodesk explain why they chose to do it this way. It just makes no sense to me.


JD,

Let me rephrase the last part. Change "without projecting them first" to "without them being projected first". I still don't see why the geometry needs to be pulled into the sketch. I'm sorry I brought that one up. It only distracted from the main question, which was about sketch orientation.


Sam,

I don't display the grid or the axes in my sketches. Too much clutter for my taste. Also, it's more comfortable for me to work with horizontal and vertical constraints. While I don't consider myself an "expert" in 3D CAD, I'm also nowhere near a beginner. I'm still relatively new to the newer versions of Inventor, though. They're improving it so fast that I miss new features and enhancements from time to time.

The bottom line here is that I assumed that the sketch orientation issue was me not knowing the proper setting to correct it. This may still may be the case. Actually, I hope it is. That way, I'll find a solution in time.


Thanks to all for your comments and suggestions,
Mike

[c.henry]

i try to build all of my models centered oarund the z-axis and in the positive side of x & y

if it is a machined part then 0,0,0 is the lower left hand corner bottom of the part thickness.

i put my geometry where i require it, I don't let inventor "place" it

really dont like the vertical and horizontal constraints.


I dont have any trouble with selecting unprojected geometry. maybe it is an app option


IV 2008
( i do have to manually place my first sketch , because i can not get the app setting to stick on the correct starting plane for me.)

[Anonymous]

Mike,

The orientation of the sketch on screen is
controlled by the UCS of that very sketch. So, here you have two options: Do not
use "Look at" tool when editing the sketch (use viewing cube instead) or
re-align the sketch coordinate system in such a way that X axis represents
horizontal orientation and the Y one - vertical. To help you to get used to this
concept quicker may I suggest you turn the visibility on the UCS icon ON in the
Options DB.

Best Regards,

Igor.

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<mikeg@goughecon.com>
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href="news:6125481@discussion.autodesk.com">news:6125481@discussion.autodesk.com...

Dennis,
There is nothing in Sketch options to control the sketch orientation. I've
tried everything, over the last several versions, and it's still the same way.
Also, the problem isn't the orientation of the view cube. I can reset it to
whatever I want. But that doesn't stop Inventor from rotating the orientation
of sketches created on the YZ plane 90 degrees CW and those created on the YZ
plane 180 degrees. I would love to here Autodesk explain why they chose to do
it this way. It just makes no sense to me. JD, Let me rephrase the last part.
Change "without projecting them first" to "without them being projected
first". I still don't see why the geometry needs to be pulled into the sketch.
I'm sorry I brought that one up. It only distracted from the main question,
which was about sketch orientation. Sam, I don't display the grid or the axes
in my sketches. Too much clutter for my taste. Also, it's more comfortable for
me to work with horizontal and vertical constraints. While I don't consider
myself an "expert" in 3D CAD, I'm also nowhere near a beginner. I'm still
relatively new to the newer versions of Inventor, though. They're improving it
so fast that I miss new features and enhancements from time to time. The
bottom line here is that I assumed that the sketch orientation issue was me
not knowing the proper setting to correct it. This may still may be the case.
Actually, I hope it is. That way, I'll find a solution in time. Thanks to all
for your comments and suggestions, Mike

[mikeg]

Igor,



Thanks for your input. I understand that each sketch has its own UCS and that I can change it. Well, I can if it's not the first sketch. As I said before, if it's the first sketch, there is nothing to realign it to. If Inventor let me align to the origin axes, that would help. But, I digress. I shouldn't have to do that at all. I hoped someone would tell me that I missed a setting somewhere, but that's not been the case.



The problem still is that Inventor thinks the UCS of a sketch on the right plane needs to be rotated 90 degrees and, even worse, why a sketch on the top plane needs to be turned upside down? I think the question has pretty much been answered, though. There is nothing I can do to make Inventor stop creating that problem. To me, it's just ridiculous and the most annoying of the everyday things I do with Inventor.



Mike



>


{quote:title=Guest wrote:}{quote}

{font:Arial}{size:2}Mike,{size}{font}

{font:Arial}{size:2}The orientation of the sketch on screen is

controlled by the UCS of that very sketch. So, here you have two options: Do not

use "Look at" tool when editing the sketch (use viewing cube instead) or

re-align the sketch coordinate system in such a way that X axis represents

horizontal orientation and the Y one - vertical. To help you to get used to this

concept quicker may I suggest you turn the visibility on the UCS icon ON in the



Options DB.{size}{font}

{font:Arial}{size:2}Best Regards,{size}{font}

{font:Arial}{size:2}Igor.{size}{font}

[segspider]

Mike,

I'm sure that any Inventor user would have similar complaints starting to use SW. It's all in what you're used to. The solution to your first problem is to set the sketch to which ever plane you want to be the default.

Tools > Application Options > See attached screen shot.

Try each one & stick with the one that works for you. And as Dennis suggested, see App Options >> Display View Cube settings if you need to tweak it further.

Dennis already covered the other problem you had about autoprojecting the edges on sketch creation.

[Josh_Petitt]

Mike,



A couple of questions/suggestions:



1) go to Application Options and uncheck "Look at sketch plane on sketch creation.

2) set your Constraint placement priority to "Parallel and perpendicular"



3) Is there a particular reason you need a sketch CS aligned in a particular fashion? (We align parts to the part CS, but do not worry about aligning/rotating sketch CS).





As far as the "problem", its not really so much of a "problem" as a choice. You will notice that if you have the "Look at sketch plane on sketch creation" selected, then when you make a sketch on one of the Origin planes, then it is oriented such that the Part CS has a vector pointing out of the screen, and another vector pointing "up". This is a reasonable choice and is consistant.



My guess is that once you turn off the option to "Look at the sketch plane..." your troubles will go away cause you can just view as you see fit.

[Josh_Petitt]

>The solution to your first problem is to set the sketch to which ever plane you want to be the default.



or set to none (which is what we do). Depending on what we are drawing, we start on different planes.

[pkquat]

I'll add my 2 cents. I have to agree with Mike on this one, and would be curious to know why Inventor rotates certain "looked at" views / planes. It was confusing to me at first, and is fun when trying to explain to newer users why that horizontal line needs a vertical constraint and vice versa. I don't remember these issues when working with ProE or SW. I wonder if this is are part of the issue when redefining sketch planes. Sometimes it rotates them 90 deg which can be annoying, especially when a sketch on a similar plane has a different orientation.

That said, I am pretty much used to it now, so it doesn't bother me much.

On a side note, I think it was possible to chose which side of a plane you sketched on with ProE a number of years back. I vaguely remember that or something similar confusing a lot of people in the class.

Pete

[Anonymous]

That's what I do too.

Igor.

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<Josh_Petitt> wrote in message
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or
set to none (which is what we do). Depending on what we are drawing, we start
on different planes.

[Anonymous]

Hi Mike

For the first sketch you can realign the sketch CS
by selecting Origin Axis's from the browser. I just tried it and it works. I
agree with you that Look At tool should be a lot more user friendly than it
is.

Regards,

Igor.

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<mikeg@goughecon.com>
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href="news:6126255@discussion.autodesk.com">news:6126255@discussion.autodesk.com...

Igor,



Thanks
for your input. I understand that each sketch has its own UCS and that I can
change it. Well, I can if it's not the first sketch. As I said before, if it's
the first sketch, there is nothing to realign it to. If Inventor let me align
to the origin axes, that would help. But, I digress. I shouldn't have to do
that at all. I hoped someone would tell me that I missed a setting somewhere,
but that's not been the case.



The problem still is that
Inventor thinks the UCS of a sketch on the right plane needs to be rotated 90
degrees and, even worse, why a sketch on the top plane needs to be turned
upside down? I think the question has pretty much been answered, though. There
is nothing I can do to make Inventor stop creating that problem. To me, it's
just ridiculous and the most annoying of the everyday things I do with
Inventor.



Mike

[mikeg]

Igor,



Yea. I just tried that in 2009. I worked fine. It didn't work in the other version I work with. I'll try it again tomorrow at work.



Still, this absolutely should not be necessary



Mike



>
{quote:title=Guest wrote:}{quote}

{font:Arial}{size:2}Hi Mike{size}{font}

{font:Arial}{size:2}For the first sketch you can realign the sketch CS

by selecting Origin Axis's from the browser. I just tried it and it works. I

agree with you that Look At tool should be a lot more user friendly than it

is.{size}{font}

{font:Arial}{size:2}Regards,{size}{font}

{font:Arial}{size:2}Igor.{size}{font}

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<mikeg@goughecon.com>

wrote in message href="news:6126255@discussion.autodesk.com">news:6126255@discussion.autodesk.com...

Igor,







Thanks

for your input. I understand that each sketch has its own UCS and that I can

change it. Well, I can if it's not the first sketch. As I said before, if it's

the first sketch, there is nothing to realign it to. If Inventor let me align

to the origin axes, that would help. But, I digress. I shouldn't have to do

that at all. I hoped someone would tell me that I missed a setting somewhere,

but that's not been the case.







The problem still is that

Inventor thinks the UCS of a sketch on the right plane needs to be rotated 90

degrees and, even worse, why a sketch on the top plane needs to be turned

upside down? I think the question has pretty much been answered, though. There

is nothing I can do to make Inventor stop creating that problem. To me, it's

just ridiculous and the most annoying of the everyday things I do with

Inventor.







Mike

[mikeg]

Josh,



First, thanks a lot for your comments. Unfortunately, there's nothing new there.



1. That makes no difference whatsoever in the the orientation of the sketch UCS, it just doesn't show you what it is. I want it to look at the sketch when I create it and I want it to be right-side up, not rotated or upside-down.



2. I don't want to use parallel and perpendicular. I prefer horizontal and vertical. It's a configuration option and it should work right. Actually it does, but the sketch UCS's are screwed up.



3. Yes. All sketches should be created with the part remaining right-side up. They aren't, which is absolutely absurd.



No, it's not a choice, it's a problem. I don't have a choice. Turning off "look at sketch..." only masks the problem. It doesn't fix it. It's not a reasonable choice at all.



It's also definitely not consistent. I can create a sketch on the XY plane, which Inventor turns upside-down. If I create some geometry on that sketch, extrude it up, then create a new sketch on the top of the new solid, it creates the sketch right-side up. Sketches created on parallel planes are created 180 degrees apart. That's hardly consistent.



I've been using Inventor for a long time. This has been screwed up at least since version 5. I realize that I must forget about it and move along. Autodesk obviously doesn't think anything's wrong. Ignoring the problem, by turning off the "look at sketch..." option, doesn't make it go away.



Thanks again for your comments,

Mike

[mikeg]

I'm not just starting to use Inventor. I've used both SW and AIS for several years. I love and hate both of them at different times.

I don't have a problem with which sketch is first. I have the automatic sketch creation option turned off altogether and have for several versions now, since I first started using Inventor. I create my first sketch myself on the plane that best suits the part I'm working with. No way that Inventor can predict that. I don't know how that got perceived as a problem in the first place. I surely didn't say it was.

Also, like I've told many others, this has nothing to do with the View Cube or it's settings. It's a sketch UCS issue. Nothing more, nothing less.

Thanks for trying,
Mike

[mikeg]

I see this discussion went away without an answer, specifically from Autodesk. I see them all over the place in these message boards, but not here.

Curious. Could it possibly be that nobody at Autodesk knows how to fix this because it can't be fixed? I'm beginning to think that's the case. Still it's absurd that they won't just admit that. They really should do one of the following:

1. Tell us how to fix this problem.
2. Tell us that they can't fix this problem.
3. Tell us that it's supposed to be that way, but include the reason why.

I don't think that's a lot to ask.

Mike

[RobertFYS]

Hi Mike,
I think you can change default template into DIN template to resolve the issue.
Steps:
1)Check on "Look at sketch on sketch in sketch Tab Creation and Sketch on y-z plane in Part Tab;
2)Select Standard(DIN).ipt as template in Metric tab,please refer to 1.JPEG;
3)New sketch,please referto 2.JPEG

thanks

Robert