Aligning Weird Angle Fittings

Sometimes, if you work out Tube and Pipe long enough you will have this problem where fittings are shown at weird angles misaligned with the run. Even if you haven’t encountered this you will at some point so do yourself a favour and read ahead on how to solve it. It is very rare when this happens and starting over your T&P layout again is always an option but you don’t have to because there’s a quick fix.

Aligned fittings

You haven’t done anything different than the usual, but when you place a fitting it comes up at a weird angle and if you try the Change Fitting Orientation command, Inventor will report “0.00” angle and so you don’t know by how much to rotate it to get it to line up with the rest of the run again.

Angles do puzzle me some times but this should be straightforward.

TIP:  The reported angle depends on the type of elbows specified in the route style, how much you drag the rotation arrows or your manually entered angle value. Nonetheless if you get a weird angle and don’t know how to align it then keep reading for a solution.

At this point you might be thinking to use the Change Fitting Orientation command and right away activate Rotation Snap on the right click menu. You will then think of dragging the arrows until they snap to adjacent geometry. Good luck with that! The randomness of getting that command to work has drove me crazy too many times.

You can also measure the angle with All Digits precision active but an almost right value is never the right value.

When I get this problem I unground the component, constrain it, ground it back and then I delete the constraints. Kind of crazy but read ahead why.

 Once you enter Tube and Pipe environment you will get customized menus, layouts and browsers so you the usual commands are not always there and for a reason I might add. While these commands are working you might brake T&P functionality and end up with unadaptive routes or even worse, crashes or corrupted files; none are fun to deal with so keep to the manual or standard procedures as much possible.

One of the missing commands is Grounded status on the right click menu, graphical window or browser. There is a reason for that, and we shouldn’t mess about with it but sometimes we have to and as long as you remember to tick it back on then we are ok.

T&P has custom menus, UI layouts and browsers.

Right click the part in the browser or graphical window, choose Occurrence tab and tick off Grounded then click OK.

Ground option is only available on iproperties.

Now you can constraint you fitting however you want it. I usually use the origin planes of the fitting and of the pipe or element right next to it.

Constrain the fitting to fix the orientation

Use the part iproperties to put the Grounded option back on and then click OK. Unfortunately there is no shortcut option to ground components but this is not that time consuming.

Delete the constraints you just created but notice that the part stays put because of the ground status.

And that’s how to align a weird angle fitting.

Later,

ADS.

TP Mixed Styles and Align 3D Ortho Tool

Let’s discuss mixed styles and aligning the 3D ortho tool for today. I am not talking about mixed flange styles but having route with both fittings and bends all in one route.
In some cases you’re having a route with fittings but for space and/or access consideration you might need a custom bend segment to be manufactured. While routing a “Rigid Pipe with Fittings” you can actually switch on the fly to creating segments with bends.
Once inside the sketch after starting the route command if you right click you will find a “Custom Bend” option on the contextual menu.

As soon as you choose Custom bend, the direction arrows change from straight to arc and 4 more arrows appear on the node. If you click on any of the node arrows, or start typing while holding your mouse over them it will change the value of the bend radius. You can do it globally not in the styles but in the parameters where a User Parameter “B” stores the default bend radius value.

Once you finish orientating the triad and you specify a distance you will end up with a fillet between your segments. This is not perfect and if you ask me when bending 90 degree it should constrain the segments perpendicular to each other and at all times the arc segment should be tangent with the straight lines but it’s not doing it. I’ve had times when the new segment was constrained to existing straight lines automatically but most of the times you need to constrain it yourself.

Sometimes these are not enough so you need to add a dimension angle between the segments and draw some construction lines to help you dimension the segment but more on that next week when we’ll cover construction lines in detail.

If your beds are 45 or 90 degrees only and you need more than one bend I would not bother to use Custom Bend especially since you need to activate it for every new segment you create. I would do my sketch as usual and then use the bend command in the Create tab of the route to add a radius between straight segments.

When you populate your route it will create straight pipe segments with fittings and sweep pipe segments from the same route.

This only works on “Rigid Pipe with Fittings” style where you have declared your fittings in the style setup, because in “Tubing with Bends” style you have no fittings declared and Inventor doesn’t know what fittings to populate.
You can drop a fitting into a tube segment and it will split that pipe segment in two separate segments.

You can also delete the arc segment inside the sketch connecting the straight segments but if the angle is not 45 or 90 (selected fittings in style) you will get a route violation, angles no permitted. If the angle is.

What’s all this got to do with aligning the 3D Ortho Tool? If you use the align command and the consecutive segments are not 45 or 90 degrees it will create a custom bend. Sometimes even if the angle is permitted by the route it will still ad a fillet for custom bend but you can remove it as described above.
If you find yourself having the 3D orho tool skewed or you want to align it to existing geometry you can do that by right clicking on the axis to align and choosing “Parallel With Edge” or “Perpendicular To Face”. This works for all axes so you can change them one after the other to an advanced align like for example if you needed to match those on the origin (check graphical window lower left corner). The colours of the ortho tool match those on the UCS origin, red X, green Y, blue Z making it really easy to do this.

And that’s it for today. Join me next week when we’ll discuss construction lines, how use them in sketching your routes faster and constrain them on weird angles.

And the video:

Later,
ADS