Friday 28 August 2015

Dimension from Route Centerlines

Quick tip today, running out of time. 

                This 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.

                Sometimes 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.

                The 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.

                And that’s it...
                Short video as well.


Thursday 27 August 2015

Tube and Pipe mixed units

 This is really a question from a YouTube friend and I have no other way of answering with images and videos so I’ve decided to share it on a blog.

The question is how to use ASME pipes with ISO 7005 flanges?  Or better yet, how to create mixed styles, mixed units routes?

2 ways really and the second is more of a cheat that I don’t recommend since Autodesk has provided a solution that is working which is to use mixed units.

+Chris Benner has documented this really nice and you can check his blog here:

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 styles.

If you have a flange that has only one column as key with the sizes then you can add another column with its alternate unit.

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.


Friday 21 August 2015

TP Branches

I’ve already showed you how I do my branched here, but I have a different solution today.

                As you 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.

                As you 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 together.

                The 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 your selection.

                Continue with Coincident Constraint by selecting the node on the fixed lines and then select the free line as your second element.

                This will in fact simulate a connection between the nodes but without generating a route violation error.

                When 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.

And the video:


Thursday 13 August 2015

Tee Coupling

I have a lovely little trick this week on using tees more dynamically inside Tube and Pipe module of Inventor.
                Analyzing 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 style.

                I decided 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.
                This 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 size.
                The main 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 around it.
                Change 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 Orientation.

 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 rotation command.
 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.

I have added the request to have Edit Fitting Orientation on the T&P Overhaul post in the idea station so here’s another reason to vote for it.
                And this is it, nice and easy with a short video as well.



Thursday 6 August 2015

TP Design Variation

Got a really nice one today.
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 ones.

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 normal.

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 itself.
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.
And the video