Tube & Pipe: Fittings not Square

[Anonymous]

Has anyone come across this before? 

my guess is that Inventor is trying to keep the Tube and Pipe Points on the tube and pipe sketch line and as a result is spinning the fitting a bit to do that. can anyone suggest a work around other than inseting and spinning it to suit? (if there is one)

[salariua]

Upload the part. I am thinking it's to do with the way it's been modeled.... but it might very well be a bug.

I had fittings dropping at weird angles before.

check Idea 51 on my page or in the Idea Station

http://blog.ads-sol.com/2015/02/tube-and-pipe-idea-station.html

[cbenner]

I've seen this before, in fact i saw this yesterday.  Are there any fittings in your line that are not tube & pipe authored?  I saw this when I placed a component into my line that was not an authored fitting, and used standard constraints on it.  My line kept rotating to something like 1.5269875 degrees.... some weird number like that.  Fought with it half the day.  Finally took the part out, derived and authored it, publishe dit and put it back on... problem solved.

So, that could be one cause, other than that, this has always baffled me.  I posted an Idea Station Idea yesterday on this as well, asking for independent fitting rotation... here is the link.

[Anonymous]

Adrian, attached as requested. 🙂 i did notice this with another fitting on another line that i had previously not had issues with though, so i went through and made sure all runs were constrained setc. noting seems to have changed. and it came good with that fitting after i placed the first one. so i will keep an eye on it today and see how i go. thanks for looking at this for me. 🙂

Chris, i am glad to know i am not alone. it is nice to finally hit a bug as opposed to stuff that i have been doing wrong. (who would have ever thought they would be happy to find a bug!!  ) until yesterday i was on the verge of giving in with this and conceding defeat. finding this first thing didn't help! i had a reasonably trouble free day yesterday though, so here's hoping for another one!

let me know if you guys have any other questions. 🙂

[Anonymous]

it's not the part. i just used it again in another run and it worked perfectly. odd that it wouldn't work at all yesterday but is fine today!

EDIT:

i take that back. if i "Place" the part it acts as per the above video. if i right click and "Connect" the part it works fine. if i right click and "Insert" the part it is on an angle......who knows?...

[salariua · Accepted solution]

Found your problem. Good or bad is for you to decide.

The orientation comes from your 3 connection points, the ones you used to author and declare your fitting engagement points. Look at the red arrow I drawn and you will get the idea immediately. This seems to be the case only when placing fittings with drop into a line (over existing fitting, node or not).

In my gif animation the red is your part and the yellow is mine. I have created another point vertical on the spool and it dropped fine (rotation wise).

What you need to do is add 4 connection points 😮 and the 3’rd is just so that you get the correct rotation when placing the fitting. You need to be careful when placing these fittings or when placing others onto this because the extra point (3’rd) we created will be available for connections. You will then end up with fittings hanging up in the air.

I have attached my part.

To be fair this looks like a bug but it seems to be intended functionality and I think we don’t see the whole picture of where this might come in hand.

[salariua]

@cbenner can you put a picture of your part ? I am just wondering if it's a similar case.

If your part is straight, then I would try and see if using Reset Front on the View Cube has any effect. Then I would look at the orientation of the sketches.

@Anonymous Come to think of it, the weird orientation might be for those not experienced enough to create a straight normal aligned model and so we're forcing an alignment if the user is not educated enough to create a robust, fully constrainted and oriented part.

[Anonymous]

Thanks for that Adrian! I am on my phone at the moment so will download the part tomorrow. But the "weird" alignment makes sense if you think about the fact that all tube and pipe needs to be exactly 90deg to each other and in perfect alignment. (Hence my assumption in the first post.) I wasn't aware that you could add a 4th point like that. (And honestly didn't think to try). will actually try that one myself tomorrow also. That is a handy trick to know. Thanks for the help.

[cbenner]

@salariua my problem was directly related to the use of an unauthored part and normal assembly constraints, inside of a pope run.  One of the constraints failed, controlling the angle of the part, and so my route went with it.