Origin Y-Axis has 0.04°-0.15° Tilt in all Projects

[ktwendt]

Hello,

I am working on some very long, straight parts (Diameter ~1.5' and Length >75') and I keep experiencing a persistent problem; my parts always end up with a tilt of 0.04° to 0.15°, which is aligned with whichever axis I have selected to reference. I have tried lofting, creating a shape and performing a circular pattern, and manually drawing the faces across five separate part files and always end with the same result. I was able to recreate the process using the following steps:

1. Create a new sketch on the X-Z plane

2. Create a hexagonal shape with an 18" diameter across flats

3. Offset plane from origin X-Z plane that is 75' above origin

4. Create a new hexagonal shape at 8" across flats using the same center point/origin center point

5. Loft between shapes (I have tried using the Y-axis as a centerline and it has not affected the outcome, and the problem still occurs without using the Loft command at all)

6. Create a sketch on any face or origin and attempt to draw a straight line from the centers of the top and bottom vertices.

Photos of steps:

1.

2.

3.

4.

5.

6. The first photo shows the departure from 90° that the part takes. The second and third photos are the bottom and top of a rectangle that I have drawn between the center of the respective vertices. The fourth photo is showing what angle appears as perpendicular. In this case, it is 90.15°.

If anyone has any suggestions to correcting this problem, I would love to hear some feedback. I am stumped. Unfortunately, I cannot upload any of my files due to company policy; but I can upload screenshots. I'll gladly provide more information as needed and try different methods. But I am fairly certain that the steps displayed above will produce the same issues on anyone's copy of Inventor. 

Thank you for your help.

[mluterman]

Check the "Angle of North" setting in the Compass area of the ViewCube (it is off by default, so you'll have to turn it on first; right-click on the ViewCube to get to its settings).

[ktwendt]

I checked it, and it appears to be unchanged in each project.

[serpennica]

i did a layout of you example. see if that works with you. inventor 2023.

where are you measuring the 90.15. i did not understand the image.

[ktwendt]

The same problem seems to happen on the part you provided: on any face, try running a line perpendicularly from the center point of the lower vertex to the center point of the upper vertex. It comes in at 89.82°:

[serpennica]

measured with Y axis and bottom surface. I get 90deg exact.

[ktwendt]

The bottom of the part has no issues aligning perfectly perpendicular to the ground. It's when I attempt to draw a sketch along one of the faces, from the very top (Y=75') to the very bottom (Y=0') that the dimension skews.

You could try drawing a 75' straight line in a separate .IPT file and copy-pasting it into a sketch on one of the faces.

I will try to find a way to record a video of my screen if this does not help.

Thank you 

[serpennica]

when doing the sketch polygon, try not to use lines that you draw. use the axis as projected geometry and constrain the polygon to that. if you are drawing the polygon and letting the mid point snap to your line the snap auto setting may not be picking up that constraint. if so then when you loft it will not be square to top loft. it may be that both sketch's have constraint problems. use dimensions to control the size. 

dimension control, and constraint (coincident) with axis (yellow line) projected.

[ktwendt]

I actually attempted this exact method and still did not have success, in either the Loft or the Circular Pattern tool. I used the axis as the center point of the hexagon, yet the faces still skew out of plumb.

[serpennica]

try to do it with a rectangle or circle and shorter distance. the polygon may be the issue.

will be offline, check back tomorrow.

[Frederick_Law]

@ktwendt 

Attach your file.

I can't find any wrong with serpennica file.

I don't understand what you're measuring.

The pole is 900.00000000".

You keep measuring less then 900" which if anything at angle should be longer then 900".

[SBix26 · Accepted solution]

I think that there is not actually an issue here.  After placing the line from center of edge to center of edge, what do you measure (with the Measure tool) between the sketch line and the bottom or top edge?

It appears from your images as if the angle displayed in the dynamic window is causing you to believe that your line is not perpendicular to the bottom edge.  But, at least in my test part, the sketch coordinate system on my tapered face is aligned with the tapered edge, not the bottom edge, and they are, of course, not exactly 90° to each other.

Try editing the sketch coordinate system before you create the line (exit sketch, right click on it and choose Edit Coordinate System).  Choose to align the X-axis with the bottom edge.

Now when you place your line or rectangle, the angle will read as you expect.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[ktwendt]

Sam B, 

I aligned the sketch coordinate system with the major axes and it seems to have corrected my problem. I'm still not sure why the issues arose, however; the faces I had selected are already parallel with the X or Z-axis, and they "lean in" the direction normal to each respective axis. Even if the sketch coordinate system/sketch face was aligned with the tapered faces, it seems like a line from center-to-center should still be at exactly 90° to the X-axis. I've attached a video to this post showing the process I had been using to measure before your solution. Either way, I appreciate your solution. Thank you!

[SBix26]

I don't know how Inventor "decides" the alignment of the sketch coordinate system on a face like that, but in this case it definitely chose the longest edge, rather than the one most closely aligned with the origin axes.

I think you can probably resolve this for yourself simply by making the model more severe-- reduce your loft length from 75' to 7.5', for instance, which will make all the angles much more dramatic.  I think that will allow you to see how the sketch alignment produces the angles that seem wrong (but actually are not).

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2