I've experienced this problem before, but up until now it wouldn't cost me a lot of time to fix. I'm hoping someone on this forum has already solved this issue; I've looked through the forum so far but couldn't find someone who already answered it.
I created a work planed defined by two surfaces, and subsequently drew a sketch on that plane.
Now, for some reason, the plane changed the "up" direction when I create a new sketch on it. In one of my models, I create a new sketch on the plane, and the model show me drawing on the bottom face, with "Bottom" from left to right. If I create a new workplane with exactly the same inputs, and draw a sketch, the default direction has "Bottom" reading from right to left.
The problem is that this affects all of my old sketches, so my entire model crashed. What was up is now down, and none of my dimensions corrected themselves.
If someone has already experienced this problem, they know exactly what I am talking about. And I experience it all of the time, since I'm using the same model for the past few months now.
Thanks a lot!
Solved! Go to Solution.
I may not have understood all of this correctly, but here are a couple of things that may/maynot help.
Use the End of Part (EOP) marker and place it under the sketch that got flipped.
Right-click on the sketch and choose Redefine, and reselect the plane.
Once the sketch is back as needed (assuming it works), use the EOP to step back down the part and fix each feature as needed (You can often use Rebuild All to fix features). At some point it will (hopefully) come back together.
Also you can right-click on the plane and choose Flip Norma, to reverse it's direction.
Will all of that said, it sounds like there is some reason this is happening, that you my need to address in order to prevent it. I'd suggest posting an example of the model in it's broken state if you can.
First, I can't realy post the problem, not sure my company would like that very much.
The normal is not reversed, that I'm sure of. It's orange on both sides.
In the past I simply went through every sketch once by one, and corrected them. Only now, the part is referenced to about 60 components (through derive).
I know there's a reason it's happening, I changed the shape of one of the surface and it must have flipped something in the internal features that we don't see. I just don't know how to change it back. I'm considering falling back to backups, but I don't recall having done one today, or yesterday..
I will try to make a new model and force it to happen, then post it.
Thanks a lot for the reply!
Okay, so it's not really a workplane that needs to be redefined but a work surface?
Did you create the surface from a sketch?
How about a screen shot of what you're working with?
I've attached a series of images (Please excuse the roughness of it) showing the current problem. I have managed to find a fix that will cause problems in the future and that only works if you catch it before the update, and that is to ground the work plane before updating. But anyone reading this can realise the potential problems with that.. (such as not being able to change it... ever).
Thanks for the screen shots, that helps alot.
I still don't understand why the workplane doesn't have a Flip Normal option? I setup a part to match what you have with the derived body, etc. and any workplane I create off of it can be flipped.
Can you right-click on the Plane and choose Redefine, as shown in the attached image?
Can you right-click on the Sketch for the feature that gets messed up and choose Redefine and then choose the opposite of the plane?
Just some thoughts, you may have already tried them, but without the file, that's about all I can think of. Maybe someone else will have a trick.
Here's a little example part I quickly made up that shows a similar problem happening when you change the original structure of the part.
Change the direction of the Extrusion from left to right and watch as the actual sketch is flipped about. Flipping the normal of the work plane may fix the problem or it may change it to a different orientation as well. Redefining the workplane may work also if you try redefining it in the OPPOSITE manner in which you defined the workplane in the first place. Meaning, reverse the order in which you select the defining faces.
Just mess around with those things a bit in my example part and watch as the sketch gets flipped around in all sorts of different positions. I understand though that your part is a bit more complex so the solution may not be as simple for this part, but without having the actual part it's hard to tell if it's repairable.
Flip normal seems to be your best bet though I think, but you could also try a combination of flipping the normal and redefining the work plane if all else fails and see if it restores the plane back properly.
EDIT: Oh, I'm guessing that you are using IV 2010, so you won't be able to open this 2011 file. Sorry. Perhaps though it will help others understand your error a bit more.
Yeah, I'm still running INV 2010.
I do have the flip Normal option; only that I need both the right orientation, and the right normal direction (so, orange facing the same side). By just flipping the Normal, some of the sketches screw up. Luckily, it's only about half a dozen that screw up, as opposed to a few hundred. No combination of redefining/flipping normal gave me exactly that I had before.
It seems that my best bet is to Flip the normal and repair the broken sketches. I would like Inventor to give the option to define the sketch plane orientation, but maybe in INV 2020...
Thanks for all of the help, both contributors. Glad to know someone was able to recreate the error!!!
See if editing the coordinarte system of the sketch does any good.
Good point. I was using the Edit Coordinate System option yesterday when looking at this issue, and noticed that after you refine an axis, you can right click and choose Flip Axis. That may be the last piece of the puzzle here.
Edit Coordinate System is acessed by right-clicking the sketch, but not when editing the sketch.
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