Corrupted T&P assembly

                Just had a couple of more crashes and corrupted T&P assemblies and I’ve decided to share the pain, or is it the fun that I am sharing, don’t really know anymore. I seem to confuse them all the time.

                As mentioned before, if you are working with T&P environment and you seem to be getting weird results it might be because of a corrupted T&P assembly. Some of the symptoms are:

-          Importing styles reports success but not styles are present (or have been imported).

-          Styles have gone missing in styles editor (none present).

-          Changing styles will not update routes.

-          Style not persistent in all runs/routes (looks different, gap, size, appearance, etc.)

-          Cannot place fittings, onto routes or freely.

-          Any other anomalies or behaviours different than usual T&P work process.

The typical folder structure for T&P is:

1.       MAIN ASM

1.1   T&P ASM

1.1.1          Run1

1.1.1.1    Route 1

1.1.1.2    Route2

1.1.1.3    ETC.

1.1.2          Run 2

1.1.3          ETC.

You’ve got a couple of choices here and you can:

-          Use a previous version in OldVersions or in Vault history. Not really an option for those that don’t use vault and the problem might be older than the backups in OldVersions.

So now what? In short you need to create a copy of the T&P assembly, or just the runs, or just the routes, depending on where the problem is.

STEP 1:

No matter what you do the first step is to create a new context for the T&P ASM.

Option 1:

Create a copy of Main ASM under a different name and that’s because we might still need the original one to save/update original files (will get back to it in a second).

Option2:

Create a new asm , place Main ASM in it and promote all components except T&P assembly. This is to maintain constraints and relations between components.

                These options are necessary, and they will create new files for the new T&P asm, as well as all the runs and routes. I would use option 1 because with promote/demote you lose constraints of the main asm, as well as any modifications in the asm, like parameters or representations (view, position, lod)

STEP2:

                Recreate the T&P asm in the new context

                Option 1:

                - Use pace component and place the original T&P assembly here.

                - Right click on it and select “Make Adaptive”. This will create new files (copy) adaptive and activated as T&P type editable files. Make sure you have “Make all runs adaptive” ticked.

                You will lose all references and included geometry for your routes but at least you will have all files created as new in the closest possible configuration to the original one. It’s just a matter of re-constraining the routes, and re-projecting your references with “include geometry”. If the T&P was corrupted sometimes in the copy process it takes the errors with it as well so check next step.

                Option 2:

                If you still have problems with T&P then you need to repeat Step 1 and instead of placing the original T&P:

                - Create a new T&P from the Environment/Begin/Tube and Pipe.

                - Save main asm (top level)

                - Not necessary but I do go back inside T&P and delete Run1 (automatically created)

                - Use place component and place the original runs. They are asm files as well and they look like this: 150122-05.Run01.iam

                - Save main asm (top level)

                - Back to T&P and right click “Make Adaptive”

                - Repeat for all Runs.

Option3:

If you have problems with one of the runs, then:

-Recreate Step1:

- Start a new T&P environment.

- In the newly created route use place component and add all the fittings and routes in the original run.

- Do this for all runs.

- Save the main asm (top level)

- Make them adaptive.

This is the longest and most frustrating, repetitive, time-consuming option but it’s here just in case some runs go bad.

               

Things to consider if you experience corrupted files lot of times:

-          Keep the T&P template in Design Data folder clean. Don’t add any styles to it, don’t edit it, this will help you when migrating to newer versions of Inventor. Have the styles exported as xml and import them when needed in your current project. Don’t import them all, just the one you are going to use

-          Make sure you have all libraries attached to your project.

-          Keep styles consistent with Content Center (no missing libraries, corrupted family tables, proper authored pars, etc.)

-          Don’t have long folder paths. T&P as well as Design Accelerator and FEA tend to create long file paths, so keep your projects as close as possible to root drive so you don’t overpass the MS Windows limit of 256 characters.

And a short video:

 

                

 Till next time,

 

Tube and Pipe 3

On first and second part we have discussed, naming and constraining your tube and pipe assembly, projecting the run planes for route constraining and importing styles so we don’t mess about with the default template.

The next thing I like to do while inside my route is Import Parameters. You don’t have to follow all this steps and I understand it might seem too much for doing a small route but it’s better to install these habits one at a time and stick with the ones you really need (find useful). I can’t help but do them all no matter how small the assembly. When you have all the time in the world to design a spool you don’t need these but when the day comes hot and heavy you will find them useful.

 What do you mean by saying Import Parameters from xml? I have a set of parameters with same name but depending on the pipe size they have different values and different description.  These are just measurements I’ve done on my fittings (most commonly used ones) in order to see how much space they take. This will help in tight confined spaces, as well as keeping the routes visual appealing.

These are the parameters that I import for a DN32 PVC-U route.

I have a set of parameters for each size-style. For DN32 PVC-U one xml file, DN32 PVC-U DN25 another xml file, DN32 ABS a different one again and so on. I use these parameters to dimension the distance between the nodes, based on what fittings I will have on the node. 

Ex: Ball valve after an elbow will have the distance between the nodes as “=e+vb+gp” (elbow parameter + ball valve parameter + gap parameter) or because it’s so common I have another parameter “ebg” that holds this sum as a formula “ebg = e+vb+gp”, so in this case I will type just “ebg”.

Unfortunately, when dynamically entering dimensions by typing the value (while holding your mouse over a reference), you can’t enter any text value so you won’t be able to type “ebg”. You can start typing a number and then in the dimension value dialog type “ebg”. Inventor will calculate the value but will not put the equation in, just the end result.  So when you edit the dimension (if you used auto-dimension) you will see the end result as 95mm instead of “ebg” what we wanted.

That’s why I just place nodes by clicking a couple of times in the desired direction and dimension right at the end using my parameters as values. If you don’t care about your dimensions, don’t bother doing this, you’re better off skipping and dimension by the “eye”.

When you start, after you select your first point (circular edge, or point) an arrow will show up indicating the direction of the route. You can change the direction either by pressing space bar or by typing a negative value while holding the mouse over the arrow vector. Because Inventor projects the plane of the circular edge and dimensions to a plane can have a negative or positive value, you can switch direction with negative sign. 

        You can enter dimensions by using right click on the reference, triad, start vector, or any face or plane your mouse can select. I don’t use the right click menu, I use + and – to increase the triad or starting vector and while holding your mouse over the reference I start typing my dimension.

If you need to use planes or faces as references, right click and activate point snap, and while holding your mouse over the face or plane start entering the value. 

If you type 100 it will create the segment 100 mm over the reference (more than), while if you type -100 it will create the segment 100 mm to the reference (less than). In my example I am holding the mouse over the wall face and type -100 to keep the nodes and segments inside the room. Inventor will not create a dimension from your node to the reference, but instead will dimension the length of the segment. I don’t want to auto-include geometry, references, and things that might change. If I want to dimension my node from the wall I will first use include geometry on the wall face.

Till next time,

Adrian.

Tube and Pipe 2

Continuing on tube and pipe tutorial from last week we are going to discuss the styles, and parameters that I like to have before doing any routes.

So you’ve started the tube and pipe assembly, maybe you gave it a name to detail it on a separate drawing, maybe not, because you are detailing it on the main assembly drawing. You have constrained the tube and pipe assembly flush on the origin of your main assembly and hopefully you have constrained the runs as well, just to make sure they can’t be dragged by mistake.

Once inside the route I like to project (include) the run planes and set them to auto-resize just in case I need some references for constraining my route. You want to use as little as possible any references that might change, making you re-dimension, re-constrain your route. If I can’t fully constrain my route by itself I sometimes use the included planes of the runs to lock it in place trying to keep it local. Sometimes no matter how many constrains you add, the route will not change colour, will not become fully constrained. If you drag the sketch from various nodes and it's not moving then leave it, it might never get fully constrained.

Now you need to look into the styles of pipe and fittings you want to use for your route. I don’t have any styles in the default template “piping runs.iam” located in the design data folder. This way I don’t need to worry about migrating my template when a new version of Inventor ships in. I had a lot of tube and pipe assemblies crash on me so this will ensure the template stays correct. I do however have preset styles that I import for each new type of pipes and runs. I have a style for ABS, PP, SS, PVDF, PVDF-HP, and so on. Each xml export has all the sizes available for that style, so I don’t have to import 1” and 2” ABS, all the possible sizes for ABS are imported all at once.

 I need to specify that the pipe length and increment in each of my styles have a really small value like 0.001 so that I can have consecutive fittings at different angles one after the other. This helps with fittings that have an exact engagement like “to point / plane”. The engagement percent takes into account the pipe length increment. The bigger the value, the more you will end up with gaps to compensate between pipe length (min+increments) and distance between nodes (fittings) which might not be divisible by the pipe lengths and its increments.

Till next week...

Adrian.

Sheet metal imports

Let me drop a couple of words on getting flat patters from imported components. I've seen a lot of imported parts lately created in other cad packages (Catia in this case) with punches that Inventor has problem creating flat pattern for.

The secret here is to use delete face with heal on and delete the inside of the punch first and only afterwards the outside faces of the punch in a separate delete operation. You can select inside faces of all punches for your first delete face operation.

If your vendor exported an assembly with one part, Inventor will imported it as multi-body part with one body and it will complain that it can't be converted to sheet metal.

In this case you can export it again to a neutral file format and import that back or you can use derive to get it all as one body.

I have a test model for you made with Inventor 2014 where you can try these out.

When you try and convert to sheet metal you will see that inventor complains about having multiple bodies so we need to derive it into a single body.

1. Open a new part.

2. Go to 3d model / create/ derive and browse to our file : 141017 Sheet metal imports.ipt

3. In the derived part dialog, expand solid bodies, and unmark Body.1 (you only need to have Body.13)

4. On the derived style select single solid body and click ok.

Even though we have only one body it seems that the round inserts at the end of the arms are modeled in so we need to remove them to a constant thickness part.

5. Extrude-cut the sheet metal nuts (round inserts)

6. Select the inside faces of the punches, one at a time or all at once. Start the delete face operation and after marking heal option click ok. You should have something as in the images bellow.

 7. Repeat the operation again for the outside faces of the punches. The end result should be like this:

 8. Verify the thickness and change it accordingly in the sheet metal options.

9. Use flat pattern. You might need to select one face (inside face) before flat patterning if it doesn't unfold. You might also need to delete the existing flat pattern if any to get it to compute.

And of course a video.

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