Need help creating a work plane facing the right way!

[bbonner]

I'm in the context of an assembly trying to add machining cuts to a cylindrical tank.  I have created work plane on the tangent surface I will be cutting. When I try to sketch on that work plane the sketch orientaints so my sketch is facing away from the object.  How can I flip the work plane so my sketch is facing the object so I may project geometry?

[mdavis22569]

I'm not sure if you have 2 questions or 1 ...

Are you automatically rotating to view when you put a sketch on a workplane and you'd like to turn that off?

The other option, that I'm not sure you're talking about is Flip Normal. If you RMB on the Workplane you can flip it.  Yellow Front/Blue back side ... flip normal will switch it...

[BeKirra]

I am afraid that you have to flip the plane before creating any extrutions on this plane.

Just in case if I misunderstood your problem here is a screenshot showing the "flip plane" method.

[JDMather]

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@BeKirra wrote:

Just in case if I misunderstood your problem here is a screenshot showing the "flip plane" method.

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I do not get that option in Inventor 2015.  What version of Inventor are you using?

Are you sure that is an assembly level workplane as described in the original post?

Or is that really really a part level workplane?

[mdavis22569]

2015 Part mode is where I did it.  

[JDMather]

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@mdavis22569 wrote:

2015 Part mode is where I did it.  

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The first sentence of the original problem description clearly lays out assembly level workplane.  The OP seems to be well aware of part level Flip Normal behavior from what I read into the problem description.

The OP even did search here before posting the question.

http://forums.autodesk.com/t5/inventor-general-discussion/flip-normal-in-assembly/td-p/3542398

[mdavis22569]

Guess I looked at "the context of an assembly" ...differently and thought he might be editting in place on a part within an assembly due to the projecting of the geometry ..

[BeKirra]

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JDMather wrote:

I do not get that option in Inventor 2015.  What version of Inventor are you using?

Are you sure that is an assembly level workplane as described in the original post?

Or is that really really a part level workplane?

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Sorry to OP & JDMather, I rushed out for an urgent job when I started writing the post.

I did not realised that the issue is about an assembly model.

To OP, in this case, the work plane cannot be flipped. And you may add a request in "Inventor IdeaStation".

[bbonner]

Hello!

In my last post, I did learn that there is a difference between work planes used in a part enviroment and a assembly enviroment.  My problem is in the assembly enviroment.  As I explained before "I'm in the context of an assembly trying to add machining cuts to a cylindrical tank.  I have created a work plane on the tangent surface I will be cutting. When I try to sketch on that work plane the sketch orientaints so the object is in front of my sketch plane and my sketch is actually facing away from the object.  How can I flip the work plane so my sketch is facing the object so I may project geometry to constrian to?"  I have also learned that the way to control an assembly work plane is by the constraints.  This work plane was created as a tangent work plane, therefore the only constraints I have are a tangent and angle constraint.  Editing the tangent constraints only puts it on the opposite side of the tank.  The angle constraint is at 0 degrees (default), changing it to 180 degrees has no effect.  Attached is a screen shot.

PS.Sorry for the new post, but I'm new to this and didn't know how to reply to the original discussion.

Thanks!

[Anonymous · Accepted solution]

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@bbonner wrote:

...This work plane was created as a tangent work plane, therefore the only constraints I have are a tangent and angle constraint.  Editing the tangent constraints only puts it on the opposite side of the tank.  The angle constraint is at 0 degrees (default), changing it to 180 degrees has no effect...

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That's tangent and angle constraints for ya. A cocktail of potential erroneous behaviour, in my opinion.

How vital is the angle constraint? Are you intending on moving the machined features if needed? Also, with tangent, is there any chance your part will change in diameter? If neither of these are true, just offset a work plane from an origin plane by the distance of the radius of the part.

Alternatively, you could create the plane you need at the part level where you can define it through a sketch (FAR more reliable) angularly and tangentially (with respect to the OD as it changes) and then just slap your assembly plane on top of it to create your machined features.

I guess I'm also a little confused as to why there was an issue in the first place. It seems to me that the first time around, you created the plane and a sketch on said plane but were blindsided by how the view rotated to look at it. Correct me if I'm wrong but that was my impression. If that's the case, rotate back around to the orientation you would like to view it from, draw your shape, create your features making sure that they are going in the appropriate direction and boom, you're done.

Am I wrong about the ability to flip the direction of a feature in an assembly? I know some of you experts out there have that answer off of the top of your head, I'm about to be in a meeting so I can't really explore it right this second.

Hope this helps!

[mdavis22569]

 I'm a little confused at what you're asking .. can you give a model to look at?

Also are you talking about the moment you place the sketch on the plane the view etc all rotate to look at the sketch ... is that the issue?  If so turn that option off... 

[SER4]

I really wish there was a Flip Side button...i.e. for tangent work planes, it would move the plane to the other side of the tangent face (e.g. a cylinder, there are two sides that are tangent & parallel to another plane).

[SBix26]

Don't recall ever having a problem with a tangent workplane on the correct side.  Can you post a screencast?  If not that, attach a file and give detailed instructions for where you're trying to create a tangent workplane.  I'm guessing that a case that is difficult/impossible would be of interest to Autodesk developers.

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Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn

[SER4]

Creating a tangent parallel workplane is easy enough to pick whichever side...however, editing it to move the plane to switch sides of a cylinder (say from the east tangent side to the west tangent side, when axis of cylinder is up) does not appear possible.

Now someone will probably say "just make a new plane on the correct side and redefine the feature)...well yeah that's a tedious option, I guess--especially if there's children feature relationships, it could blow up pretty quick.

FYI, the reason for wanting to switch sides is if I can't decide yet which side I want a feature to be (might depend on other things, etc.)  The assembly tangent constraint already has the ability to solve 'inside' or 'outside'.

[Anonymous]

So I'll be honest, I never use tangent planes. It's just a personal thing with inventor that outside of a sketch, you'll never find me telling anything to be tangent. It always seems to cause more problems than it solves (in the long run).

All that to just say I don't have a ton of experience with them and can't say for sure that there's no way to do what you're wanting to do as it pertains to strictly working with tangent planes.

There are, however, many other approaches to achieve a similar result. Especially if this is in a part file. And I think you could probably redefine your current plane to use a different definition method and maintain your current results. I cannot, however, speak for what may happen when you try to switch from east to west. That all depends on the remaining features and how many references there are to the feature you wish to change. That can be very touchy and can sometimes require a careful hand if you intend to have something change on the fly.

There are two ways I'd suggest approaching this personally:

A) Create a plane that rotates around the cylindrical axis by whatever angle (reliable in part files, less so in assemblies). Then offset a plane from that by the radius of the cylinder (best to actually use the dimension that defines the feature rather than just inputting a number just in case.. something changes). The offset plane may just be the redefinition of the plane you're currently using.

B) Assuming you have a sketch with a circle somewhere that defines this cylindrical face (or that you can create one that references it), this may look like two circles concentric on a plane that are used to extrude a pipe for example. You can create 2 construction lines from the center point out to the edge: one should be constrained to the origin axis (vertical or horizontal) and the other free to rotate. Then create an angular dimension between the two. The plane definition comes from selecting the rotating line and then it's endpoint on the edge of the cylinder.

Both of these methods should create a plane that will stay oriented properly with respect to the cylinder and allow you to move the plane and accompanying features to suit your needs.

This is just what I would do though. It's a little extra work compared to telling a plane to be tangent to a surface but I find a little more time for a more robust and/or flexible solution always pays off in the end.

Hope this helps!

[johnsonshiue]

Hi Folks,

This is about how Inventor infer the coordinate system from a selected face. There is room for improvement for sure. Before a solution is found, I suggest you use UCS to have more predictable plane orientation.

Many thanks!