Deleting Fittings

                Deleting fittings can be daunting and you can end up spending hours in rework. If ever struggled with this then problem you will be happy to know there’s a trick or two to bypass this limitation (bug more likely).

All fittings CAN be deleted, just need to know how.

                Usually as you select a fitting you will get Delete option on the right click menu but every once in a while, just when you need it most and you are in a hurry, rushing a deadline you find this missing option. You probably hope no one will see a fitting floating around or as an advanced user you are, you turn the visibility off for the component in the design view presentations or turn the line visibility off in the drawing.

Missing Delete option on the right click menu.

                Not to be finger pointing, but I had someone turning the color of the lines white on the drawing in his need to hide/delete a fitting. This tricked the drawing aspect but not the prints and exports.

                You will more likely see this bug when you copy/paste a fitting in the browser or graphical window. I tend to do this when I need a copy of an existing fitting with a different size. For some reason the new fitting will lose part of the TP functionality (icon on the browser will not be a blue tee icon specific of TP fittings). At this point you cannot delete it unless you select it and then press delete on your keyboard. There is no delete on the right click contextual menu on the graphical window or browser

                If using “Delete” on your keyboard is also not working, the trick is to use demote, promote to a point where delete gets active and you can use it.

                Select the fittings in the browser and drag them outside T&P assembly. Then step at that level and notice that there still is a missing delete option on some/all of the fittings. Select them again and use demote on the right click contextual menu (under Components) or press “TAB” on your keyboard.  

Drag / promote fittings.

                Don’t worry about giving a proper name and a save location for the new assembly. We will never save it but instead, as soon as the fittings are grouped under this new file select it and press Delete key or use the right click contextual menu.

 

Still missing Delete? Demote them...

 

How's this working then?

                In the next post will be covering broken links for fittings that don’t update with the route and for some reason they remain in the assembly. While the fix is similar there is a catch on how to get that route to populate again and save recreating the route.

Delete key worked but here's promote/demote. 

Later,

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photo credit: Selection (license)

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

Later,

ADS.

Inventor TP Trim / Extend Pipe

Last week’s post again. I have been absolutely buried with work and it’s seems it will stay like that for a while. Had it all prepared, I have sketched the blog and done the video and then it all came rumbling down and got buried. Now that I am back into the light have managed to upload it and get it published.

It seems the word is out....I am busy editing the last edition of Mastering Inventor 2016 by +Paul Munford (Thank You, Paul)

http://cadsetterout.com/mastering-inventor/ 

 

Tube and Pipe once more with a nice trick about trim / extending your routes. I have been working on a good example and decided to share the info on this post and this time… a video! 

I have been working on this container and there wasn’t a lot of room so before I even knew all the details like the size of the pipes I have started laying my routes and prove that it fits.

But in the process I haven’t used any fittings like flanges and couplings just rather ran them straight from the equipment to the container termination points. The problem is that the pipes will be flushed on the equipment without giving you any gaps for the matching fittings. 

In my case I am trying to place a flange but it will be connected to the pipe and therefore interfere with the tank matching flange. You can edit the connection and specify a negative value but I choose to place the flange with “connect fitting” straight on to the matching flange of the tank. Now the pipe will interfere with your flange but the fix is easy and it became the main subject of this post.

 

Inside the route if you right click on the route end node you will get a Trim/Extend Pipe option. This will only be available for an ending node and if you try it on a middle node you will see it’s grayed out.

TIP: If you have populated the route and you right click on a node you can see if it holds a fitting or not but checking if there is a check mark in front of the “fitting” on the right click menu.

I am entering a value of 5 mm and choose trim option in the pop-up window and then finish the route. You will notice that the route hasn’t changed and it’s still connected to the tank flange but the pipe has been adjusted and it’s smaller by 5 mm.

This will allow you to adjust your routes and get better, more accurate parts lists as well as proper fabrication drawings.

As promised here’s the video.

Later,

ADS

Tube and pipe construction lines

Last week I’ve shown you how to do mixed styles routes and how to align the 3D ortho tool and now it’s time to discuss construction lines for Tube and Pipe module of Autodesk Inventor. At this point I wonder how many of you are using them and even know of their existence?

The place command is hidden, you cannot change them to normal and vice-versa, they are always visible in the model and drawing and yet there are times when you might need them.

Can’t say I blame you if you’re not using them, you can do away with just dimensions and constraints but I found them useful at times and that’s why I decided to share this post.

They could be annoying being visible all the time but you can hide the route if need to and on the positive side you can edit the route really quick by double clicking on the visible lines.

The command is not on the ribbon and it can only be invoked by right clicking on a node inside the route. This is only available for route nodes, not on construction line nodes, and it’s only available in the contextual menu while you are in the main Tube and Pipe environment. If you open the run on itself and try to edit the route you won’t have the option to do construction lines.

                               

On each node you can start multiple construction lines but keep in mind that you need to constrain them even though you used the triad axis when drawing them. Regular segments get constrained at least collinear or perpendicular with previous segments, while construction lines are floating in model space with just one end connected to the starting node.

In the image bellow I am constraining the tee center in between the pumps by first creating a construction line from one pump center to the second. Then I am doing a different line starting from the tee node perpendicular to the first one and coincident with the middle of first one.

                                 

A more eloquent example might be when you need to dimension you route at an angle for which you can’t use included geometry. At this point you can’t add dimension between segments and planes, just to nodes and to get it right you might need to play with formulas and trigonometry.

                                              

Using construction lines you can constrain the projection of the angled segment into a plane that suits you where dimensions can be applied.

As you can see in the image bellow I have created a couple of construction lines to serve as projection of the angled segment. There is a third one that is constrained against the run origin (included geometry) and is used as fixed reference to dimension against.

                                               

  

In the last example that I have used construction lines to form a grid to which I have constrained my nodes. This will work similar to reused dimensions but it’s less messy, and the route is a little neater.

Start a construction line and constrain it to your references, I would recommend that you use include geometry on run origin planes. Keep your external references to a minimum, try to avoid faces that could change leaving you with broken links. Keep these as local as you can just like my run planes.

Constrain this construction line coincident to one of the points, it doesn’t need to be the farthest away, and you could even just use a small dimension to minimize its visual impact outside of the route. Coincide the rest of the points that lay on this line even if it doesn’t passes through them. The points will be in line with the construction segment.

At this point you just need to dimension one of the nodes and the rest of them in-line will follow.

The good part is that Inventor doesn’t generate a pipe segment where you’ve used construction lines but you can’t switch them back and forward as you might expect. Once you’ve done it as construction you need to remove it and draw it again as regular if you need a pipe segment there.

The drawing environment is having the same visibility problem with this type of lines. As soon as you use include route centers it will bring over the construction lines as well. You then need to turn visibility off by selecting them individually or with window select.

And that’s how you can use construction lines to help you speed up your design.

As usual, there’s a video.

Later,

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