One LOD To Rule Them All

NEVER use more than on LOD (Level of Detail) in the drawing, especially for large assemblies.

I see this problem ALL THE TIME, new or experienced users so, even if it’s not a proper blog I need to get this out… you all need to know, understand and remember this.

LOD is a memory tool not to be used in the drawings. Each LOD will load in to memory all the parts as if they were new parts even if they are just occurrences (duplicates).

Say you have an assembly of 1000 parts and you create a LOD where you suppress 1 element. If you use these two LOD’s on separate views in the same drawing then the number of occurrences will be 1000 + 999 = 1999 instead of 1000. Inventor treats each LOD as a separate assembly in the drawing!!!!

You will see a huge increase in size and you will impact performance severely.

Use Design View Representations to document different views and if you need to use LOD then have one per drawing (all sheets) like “All Content Center Suppressed” and differentiate the changes with Design View Representations.

                Now you can filter Parts List for “Design View Representation” and document a specific configuration on each Parts List but the Quantity will come from the full assembly (2017 has a fix on this).

                For now, to fix the quantity you need to look at iAssemblies. My notes on this here.

                Take a look at Large Assembly Instructions.pdf.

                You might want to suppress some of the views and turn them on when you need to work on them.

Now, repeat after me: “I swear to use only one LOD for each drawing, cross my hart and hope Inventor crashes if not”.

Later,

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photo credit: Vanishing Point (license)

Documenting tube and pipe spools

+Paul Munford has been keeping me really busy so I didn’t had time to update the blog in 2 weeks… way too long.

Last time we were discussing reordering tube and pipe components, more exactly the lack of it and I have asked you to vote for this request on Autodesk Idea Station.

Meanwhile I have been trying to find some solutions on my own and I have taken a clean approach controlling my urge to search the internet for existing solutions.

In parallel I have been asking Autodesk to give us a way of converting a route (ipt) into a regular part that we can use outside T&P. At the moment its’ not possible but CAI from Adesk has given us a code that does 90 percent of the job done. However I am still testing this solution and it was all too big for a single video, single blog so it’s on for next time hoping it will become a valid solution for this problem.

First of all: What is a spool?

We call spool an assembly of pipe and fittings like elbows, flanges, tees, etc., usually terminated with flanges. Piping systems for process plants in general are commissioned into two stages: the pre-fabrication of pipe spools and the site installation. Some of the reason for pre-fabrication are limited space on site, weight of components, weather independent production, better quality, higher accuracy etc. On the down side they might not fit on site but all things considered spools are widely used throughout the industry.

My background is high quality, high purity water for medical, pharmaceutical and scientific industry so I don’t deal with spools at all but Autodesk is really slow at improving Tube and Pipe and I wanted to test the water and see what I can come up with. Decided to see what’s out of the box, ignoring ilogic and other vb scripts that could solve this mess.

In an ideal world you would have each spool as a separate run so that BOM and Parts List will indicate proper quantity but it’s not feasible to do ten thousands runs in a single T&P assembly. Keep in mind that due to its weight a spool can be just a flanged tee (think large diameters).

On this premises I would do the whole T&P in a single Run, mingle them all in and control the sizes by creating separate routes.

First solution: Design View Representations.

I bet you’re using this right now and there’s nothing new under the sun but I will present this anyway because there might be some nice tricks you’re not using at the moment.

I like to do my design view representations and level of details in a separate tab so open the assembly, locate the run and right click open. For simplicity I will call the assembly that contains the Tube and Pipe assembly “Main Assembly”.

TIP: You cannot create a design view from within the main assembly for the T&P assembly or any of its runs so if you want to modify design views you need open the files explicitly.

  TIP: Saving runs is only possible form the T&P assembly or any level higher but as long as they are both open you can modify the files and then switch back to the T&P assembly or any level higher (like the main assembly) and save the changes.

TIP: There is no Open option when right-clicking a route in the browser so if you need to open it you can select it in graphical window or the browser but right click on the graphical window to find the open command.

With the run open expand the Representations folder, right click the main view node and choose new. Click twice on its name to change it something more meaningful. Select your spool components and choose isolate from the right-click contextual menu.

TIP: To quickly choose parts at any level down bellow hold down SHIFT and in the right click menu choose Part Priority. Now you can select any part no matter how deep it is buried in the level tree.

TIP: Another way of isolating components is to select them and then hold SHIFT+right-click and choose invert selection to select all other where you can toggle Visible off.

In the drawing environment when placing the view select your design view previously created to bring in a and display just those components.

The main problem with this solution is the reported quantity and item number in the parts list.

While place a parts list for your view you will notice that all parts are shown but we can overcome this with a filter. Edit the parts list and choose Filter Setting, and in the Define Filter Item drop down menu choose Assembly View Representation. In the view representations choose the one you defined, click the green checkmark then OK for the Filter Settings window and OK again for Parts List window. Alternately instead of filtering for Assembly View representations you could filter for Ballooned Items. The parts list will be empty until you start ballooning your view and you will end up with same results only that you need to have balloons for each item you want to show up in the parts list.

You will notice that the quantity and item number will take into account the whole assembly and furthermore the item number might be out of sequence. You can use the renumber items function on the parts list but only if you detail each design view on its own drawing. The item override is drawing persistent so creating separate sheets will not work, and the changes on one sheet will modify all sheets so you will end up with weird sequencing or duplicate item number.

As long as you inform your fabricators that the quantity and the item number pertain to the whole project you might want to use this solution.

Second solution: iAssemblyes. (I can hear some eyes popping out).

Creating iAssembly members is another way of documenting the spools and with better results. Creating iassemblyes is not possible while editing the files from the main assembly and once again you need to open the files explicitly.

Right click on a run in the browser or graphical window and choose Open. On the Manage tab, Author panel click Create iAssembly. This will create configurations of the run where each member will be a separate file on disk. Right click on the Member column and notice that it’s marked as the filename column. Specify different names for your members but you can have same part number for all of them. Right click anywhere on row one, choose insert row and setup your part number and member/filename values. Click OK when you finished adding rows.

TIP: Use the Options button to setup sequencing and auto fill in for your member, part number values.

Once you close the iAssemlbly Author window you will notice a Table in the browser right under Relationships folder. This will contain all the children listed by the Member name. If you right click on the Table node you can choose:

-Delete (this will convert the ipart/iAssembly to normal)

-New (to create a new member)

- Edit table (this will edit the table inside Inventor)

- Edit via spreadsheet (will open in excel)

If you convert the T&P assembly or a run to iAssembly, the Edit table option is grayed out but all the rest will work and opening with excel will allow any operation like deleting a member.

TIP: If you want to edit the table inside Inventor you can click on Create iAssembly again from the Manage tab and it will bring up the table editor even though the option is grayed out in the browser contextual menu. Also, instead of creating the T&P files in the main assembly you can create another subassembly in between (a container if you will). The edit table will be available in here from the contextual menu or by double-clicking the Table node.

As a general rule if you have 3 spools then you need to create 4 members. The first member you will keep intact and it’s used to show and document the complete assembly while the other you will modify to show individual spools.

In order to modify a member alone without changing any other you need to activate the Edit Member Scope in the Manage tab, Author panel, Edit Factory Scope fly-out arrow.

Activate the second member and after selecting all the components that are not part of the spool choose Exclude from the contextual menu.

TIP: You can do that really quickly by choosing the spool parts and then hold down SHIFT + right-click and use Invert Selection. Now you can click Exclude from the contextual menu.

Do this for all spools and then save the file.

Open the drawing and place a view. In the Drawing View place dialog switch to Model State tab and choose the member you want to detail then click OK to place the view.

Placing  a parts list from that view will populate the table with only those components in the correct quantity as well. In the edit table window you can choose a different member to report by clicking the Member Selection button. Here you can also notice that Hide rows of zero quantity is checked. This is what hides the other members so keep it checked.

You can show the number if items by adding Item QTY to your list from the column chooser menu but DO NOT REMOVE QTY from the list while in here because the Parts List will show complete assembly again. Click OK in the Parts List Column Chooser and then right click the QTY column and select Column Width. Here enter a really small value like 0.1, click OK to accept and then Apply in the Parts List window.

This will hide the QTY column from the Parts List but depending on where QTY column was in the editor window you will see a double vertical line that you can drag left/right to show the column. Applying the changes will show QTY column in the editor window but not on the drawing.

TIP: You can zoom the editor window just like in any other program (adobe, web browser, explorer, office products) by holding down CTRL and spinning the mouse wheel up and down. This will make it easier to show the QTY column again.

So now we have proper items reported with a proper quantity but the item number is still out of sequence. Just like in the design view solution you can use the Renumber Items function in the table editor. Keep in mind that these are drawing specific so you need to detail each spool on a separate drawing rather than on separate sheets.

And this is it…. Are you still awake?

Like I have mentioned I am still experimenting with a different solution and I found a few bugs that need documenting. I hope to have it ready for next post.

Video to follow..

Later,

ADS.

Inventor Assembly Template

                There is a lot of info on the internet on how to setup your template files and many of you have already configured the drawing template, adding title blocks, borders and some symbols maybe. You have probably edited the part template and changed the default material but chances are that you haven’t altered your assembly template too much if at all.

                I am saying this because I see recurring questions popping out every once in while by frustrated people doing repetitive tasks that could have been avoided with a proper setup of their assembly template.

                One of the main things that will save a lot of frustration would be to setup a new design view representation as default instead of the locked “Master”. God knows how many times I’ve found Assemblies that cannot be saved because of the “Main design view is locked” error.

TIP: Instead of locating the template file and folder you can create a new file using New command and then save those changes in the template using Inventor (big I top left) / Save As / Save Copy As Template command.

                So open your standard.iam file template or fire up the new assembly command. Create a new design view representation, I call mine “Default” and set is as active. This will become the default view and hopefully if you don’t manually change it back to Master you should get over that pesky error on editing locked design views.

                The next one up is BOM. By default the Structured tab is disabled and every time you place a Parts List or edit the BOM you need to activate it. You then set it to All Levels, you may change the default delimiter and most certainly you will add and remove columns to suit your design needs.

So why don’t you go ahead and make these changes persistent in the template?

Depending on your design process and needs you might not use this but I recommend that you add Item QTY to your BOM. This will report the cumulated number of instances in the BOM. The default QTY will report the number of items as long as the item doesn’t have a length (G_L parameter) like structural sections, pipes, etc. in which case it will report cumulated length and not the number of items in the assembly.

                I feel better already, anything else?

                I use a lot of Content Center and Purchase Parts that are library read-only items and when doing large assemblies it’s hard to navigate the browser to find that part you want to edit. So what I like to do is add two folders called CC (Content Center) and PP (Purchased Parts) where I group the files to clean up the browser keeping just the normal parts. It makes a huge difference to be able to find something fast not to hunt and pick all the time. Also, you can now suppress hide or disable a whole folder at a time ;)

                Nice... what else?

                How about adding some virtual parts? This is where you get creative and to utilise the tip above you might want to add them to a folder called Virtual. It’s better to add as much you can think off and then delete them in the assembly later if not used. Creative? Like what? Stuff like oil, grease, man hour costs, machining costs, shipment, painting, etc. Remember that you have Estimated Cost on iproperties and virtual parts although exist in the assembly only they do have iproperties just like any other parts. You can even add a long descriptive text in the comments field. Do you need to add the Estimated Cost to BOM? How about Comments then?

                Keep going please!

                 Anything you need changing in the Document Settings? Maybe you want to change the default Lightning Style, maybe not but you might want to change the default dimension display to “Display as expression” to see the full equation driving that dimension. In here you can change the units as well as modelling precision. Verify all the tabs and make sure there’s nothing else that needs changing.

                Is this it?

                On the short list you might also consider:

·         Deactivating the Contact Solver in Inspect Tab

·         Parameters that you keep adding all the time like bounding box dimensions.

·         Link or embed some excel files

·         Add various iLogic Forms if needed

·         Add some iLogic code like one to prompt you to fill in iProperties at first save.

·         Turn on Center of Gravity

·         Etc.

I suggest that every time you find yourself changing settings in an assembly pause and think if this is something that might be saved in the template. If you do this for a week then you’ve probably got most of things but it’s a good exercise to do every once in a while especially with each new Inventor release.

               

Later,

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