is more of a continuation of this post, where I’ve shown you how to use the
trim/extend pipes in Tube and Pipe module of Autodesk Inventor. Because I was
in a hurry and I needed to prove for fit the layout before jumping into
detailing I have done the routes straight from the equipment without adding
fittings first. In the image bellow, if you can’t remember the original post, I
have connected the tank to the outlet of the container without adding flanges,
or any other fittings and adapters that might be needed. I then added the
fittings to the equipment and after measuring how much the pipe should be cut
off I used trim on the route segments to generate proper length pipes.
when I am making drawings of pipes for manufacturing and quotes I feel it’s
better to show them as shaded views and make each run in a different colour to
better distinguish one from the other.
problem comes when I need to dimension isometric views and it’s hard to pick
the end of the flange or fitting. You can change your selection filter to parts
and then select the fitting and choose Hidden Lines. This will prompt you with
a message but you can now pick the furthermost edge to dimension against.
Now you can turn
off hidden lines and the dimension will persist but that might be too much work
for some of you. So if you’re in a hurry like I was you can route without the
fittings and then when you use “Include Route Centerlines” the dimensions of
the route will be the overall dimensions with fittings in place.
In short when you edit the style
make sure you check the Mixed Units box and then you will be prompted to select
a flange. The flange family needs to have dual units and you will notice just
like in my case for the 7005-01 flange there are 2 nominal size columns, one in
metric and one imperial and that’s how Inventor can use it in mixed units
If you have a flange that has only
one column as key with the sizes then you can add another column with its
The second one is a cheat and
almost not worth mentioning but you can copy the family to your library and
edit the key column values to its alternate units therefore it will be picked
up by the TP style dialog. I bet it will take you just about same time to do it
properly by adding a new column with its alternate units.
I’ve already showed you how I do my branched here, but I
have a different solution today.
are aware you cannot connect a third line where two are already connected and
the error you will get from Inventor is: “Branches not allowed in routes”. Well
now, we already proved that it's possible and here I will show you a different,
and in some aspects better way.
try to connect another line where two are joined into a node the route goes
into violation mode and it’s partially locked for editing until you fix this
error by deleting the segment or removing the constraints that hold it all
alternate solution is to use Coincident Constraint but not as you might expect,
by connecting the 3 nodes together. Instead constrain the node to the line
twice and you simulate a node to node constraint but without Inventor seeing
this as a branch.
Start the Coincident constraint, and select the
end of the free line. Choose one of the fixed lines for the second element of
with Coincident Constraint by selecting the node on the fixed lines and then
select the free line as your second element.
will in fact simulate a connection between the nodes but without generating a
route violation error.
you place a fitting like the tee in the line the pipes are trimmed
automatically to the engagement distance. For the free node (open ends) you can
choose Trim/Extend Pipe from the contextual menu and set a manual value. Those
of you that follow my blog and videos know that I like to import parameters
with preset values for how much space a fitting will take, like valves, tees or
elbows (in my case they take same space for installment). When I use trim on the
loose end branch line I am actually typing “ee” to get the engagement distance parameter value and to
have Inventor automatically update it when I change size of the route.
If you have already connected the free line to
the fixed ones you need to select the node and see if Trim/Extend Pipe is on
the contextual menu. If there isn’t one click the node again and in the right
click menu choose Select Other and see if there’s an option for second point,
or the third. You cannot get it wrong and edit a different pipe because only
the free end has this option and is allowing you to trim/extend.
TIP: From all my tests
Point 2 is the free end so right from the beginning Select Other and right
click when “2.Point” shows up to get the
Trim/Extend Pipe menu. This of course depends on your selection order when
doing the coincident constraint.
TIP: Sometimes when
populating a route it will complain that it’s intersecting with itself and you
need to edit the route and allow for gaps before connecting the points. This
goes against my rule to populate the routes at the very end but the solution is
to create a small segment, step up and populate and then remove the segment and
do your normal routing. The error only occurs the first time you populate a
route. If the route has been populated once it can run intersect it as much as
you can and you won’t have an error.
I have a lovely little trick this
week on using tees more dynamically inside Tube and Pipe module of Inventor.
the way I do my routes I noticed that most the fittings I place split into tees
or other fittings(like valves, clips,
reducers, etc.). I almost never use a connector, a union, or coupling. We use
unions and not couplings because they can be disconnected and they are not a
permanent connection so we have unions in the Coupling section of our T&P
to change the union for a tee in the style dialog so each node will have a
tee by default and I can drop a different fitting on it if needed (valve, clip.
etc). We use tees for sample valves, pressure gauges, branching, or any other instrumentation
like transducers, switches, quality indicator and transmitters.
will have one main advantage instead of placing tees manually and that is the automatic update and change of size for the tee. If
you place it manually and you change size of the route the tee doesn’t change
disadvantage is that there is no edit fitting orientation for parts specified
in the Tube and Pipe Styles window and for a tee that’s unheard of. So the
tees will have locked orientation ... or NOT because as always I have a way
the Tube and Pipe Style and in the Coupling section browse for you fitting. Elbow
or else it’s all working as long as two of the connections have 180 deg between them.
As soon as you populate or update the route you will have tees in all the nodes
and if you right click them you will notice that there is no Edit Fitting
Select the tee and then use Place Fitting and
drop it on to the one you need to change orientation. You will have a rotation
and position dialog just like regular place fitting so enter your angle and finish the
If you change size of the route now you will see
that the tee has been change do custom and it will not update in size so there’s
an extra step you need to do in order to maintain size associativity. After you
rotated the tee right click on it and choose Restore Fitting. This will tell
Inventor to change your fitting (tee) with the one specified in the style
dialog (same tee) but the orientation will be preserved and the size will
change with the style.
The title might
confuse you and lead you to believe that I will talk about iAssemblies. That’s
a nice topic on its own but I will cover a different idea.
You will use this
in the prototyping phase to quickly test alternate solutions for routing your
pipes. And when you do, think of me and all the sleepless nights I’ve wasted
testing and pushing the limits of Inventor and T&P trying to help you out.
For months I have
been testing and preparing a blog on mirror, clone, derive, and copy and ...
there’s not much to be told. Autodesk has locked it all in and it’s for the
most of it unavailable so no blog for me. I am still testing though and present
the mirror command briefly in here now.
One of the posts
on the idea station on overhauling T&P (idea 56 actually) is about getting route
lines to construction and vice-versa and in the process have Inventor to
automatically add and remove pipes depending on the line type.
That is a nice idea and you should vote for
it, but meanwhile........ I have found a
way around it!
Don’t go tell Autodesk because they might fix
it, taking this option out and leave us to dry out again.
I have just
finished a quote for a client and it’s been accepted and signed off when we got
the CALL. It needs to be on the other side of the room and need it presto !
If you try to use
mirror on T&P or any of its runs you will get this message:
Maybe one of you
has a solution but I have tested as much as I could and no solution emerged. You
can mirror it alright but you can’t modify it later on, by means of making it a
T&P run and routes. If you disable T&P add-in you can use the mirror
and what I’ve done was to reuse all except routes and pipe segments. This works
so you can document it on a drawing but there is no “Make Adaptive” menu in
T&P anymore so it can’t be edited as we would a copied route.
You can however
mirror the sketch segments inside the route. This is not available on the Route
tab but on the 3D Sketch tab. This works ok and it’s better than you think. The
new segments will have mirror constrains and adapt to changes to the original
So I had a partial
solution to quickly mirror my routes but what about the fittings? Unfortunately
I had to place the fittings all again but took seconds because I would pick
them from the original route.
The problem is
that if you delete the original route segments you lose all constraints and
dimensions for the mirrored ones as well.
So I decided to
see if I can change the original segments to construction line and make
Inventor remove all the associated pipes and fittings. Using the Construction
button from the Format panel of 3D Sketch tab didn’t work at all but that’s
where we become creative and started“bending the rules”.
Let’s call the
assembly with the T&P files “main assembly” just to clear things out.
Create a new assembly and place the main assembly.
TIP: fastest way is to use copy paste. You right click the main
assembly (top node) and choose copy and in the new assembly use CTRL+V or paste
from right-click contextual menu.
Find the route in
the browser and edit it. Inventor will complain and tell you that: “To perform
Tube and Pipe operations, the main Tube and Pipe assembly should be open in its
own document”. Select the segments you need to change and use the Construction
button from the format panel of the 3D Sketch tab. As soon as you exit the
route Inventor will remove the pipe and fittings that were converted to
construction and will add elements where construction has been converted to
This opens a whole
new way of doing my prototypes and to test and verify alternate routing
solutions in the conceptual phase. It’s there where I tend to waste a lot of
time trying to spaghetti fit my pipes and the only option till now was to
delete segments and route them differently while now I can keep all options and
better test which will work better.
On a side node you
can now change all the edges added to the route with Include Geometry tool and
that were construction lines. So you can use edges from other equipment without
routing and constraining on top of them but rather use the included edge
At this point you
can close the new test assembly without saving it. It has never been saved on
disk just helped us change the route segments.