Inventor Drawings of Welded Assemblies

[AnchorChain]

Our company has very recently migrated from AutoCAD Mechanical to Inventor head first.  We're figuring things out but still have some issues.

My Mission:

I have a welded assembly of approximately 50 parts.  Each part is modeled individually with it's own unique part number.  Then I created an assembly of the parts for my weldment.  We then create two drawings "Details" and "Weldment".  The "Details" drawing is just that, it details each individual part and how to make it.  The "Weldment" is a drawing that locates all of the detail parts as a welded assembly.

The Problem:

Since I have individual parts and then an assembly I can not figure out a way to create my detail drawing with all of the parts, and have a complete parts list where all of the part numbers in the parts list are properly linked to each detail view.  We've tried this two ways:

1. Insert each part as a new base view.  Browse and select the assembly for the parts list.  When I do this all of the part item bubbles in the view are "#1" not matching, or linked to, the parts list. So then we have to go in and manually over ride each item bubble to match the parts list.
2. Someone else here is inserting a view of the assembly as the base view and then taking numerous section views for each part and turning off the visibility of the parts in the section view he does not want to see.  This accomplishes our goal of having all of our detailed parts and linked to the parts list but it seems too hard and sloppy to be correct.  Not to mention someone just opened his drawing and all of the views were mixed up all over the place.

From searching around the forum do I need to create 50 Levels of Detail, one for each part view? Or Design Representations?  It seems the consensus, is to use Design Representations.

This is one aspect of Inventor that does not seem to "mesh" with our company standard for creating drawings.  It also has be completely confused on how to accomplish this with the least amount of over riding "stuff".

[blair]

You could create the drawing for the main assembly, then add additional pages/sheets to the drawing and create your drawing views for each of the parts. You simply need browse to the part rather than selecting the default file name for the assembly when you create each of the part views. Our drawing tend to match our ERP system. If we have a part number on the system, we then have a separate file/drawing for the part. If the Part number is for a assembly, then all related component drawings that don't have a ERP part number are then only included in the main drawing. You could end up with a drawing with over 20 sheets. This putting and the eggs in one basket is great for file-keeping but should something happen to the file you can loose a lot of data. Myself I would just label the Views for each part with it's part number. If you keep the part views in some form of part number sequence to match your Parts List, most people should be able to find the correct view.

[BLHDrafting]

Congratulations on making the jump to Inventor.

You've come across 1 of the key fundamentals in understanding Inventor. It is designed so that each assy file or part file has a matching drawing (IDW or DWG) file made up of as many sheets as needed. It is not designed to have a drawing (1 sheet or more) with, for example, sheet 1 being the assy file and the Parts List and then all of the child parts of that assy detailed on the following sheets in that set. It can be done but getting Parts List Item 1 (lets say a child part) to be shown in the View Label of that part is a manual process as Blair mentioned. The Parts List represents the assy file you selected when placing the List. You can't place a Parts List for a part view (you can be it's pointless).

This is one of the biggest differences between Inventor and Autocad. While it's not a solution to your problem I hope it helps in your transition to Inventor.

[karthur1 · Accepted solution]

---

@AnchorChain wrote:

 ......

I have a welded assembly of approximately 50 parts.  Each part is modeled individually with it's own unique part number.  .....

Since I have individual parts and then an assembly I can not figure out a way to create my detail drawing with all of the parts, and have a complete parts list where all of the part numbers in the parts list are properly linked to each detail view.  

---

We went through the same thing when we first started using Inventor.  We wanted our Inventor drawings to "look" like the Autocad drawings with all the part details on a single sheet with the Wledment Parts List.  It is no problem having the parts list on the sheet (just place the parts list and choose the iam).  It is also easy to get the details spread out on the sheet.  The problem is getting the item number for the parts list to correspond with the part detail.  I could never accomplish this because the item number is not a selectable property in the format text window.

The best that I could do was to change the view label for the detail to include the part number  (see below).

We have gradually migrated to the one-sheet,one-part,one filename workflow.  We have the part details on a single sheet, the weldment on its own sheet.... etc.  It is much easier this way for us.

Kirk

[nmunro]

Although one part - one drawing is generally the best approach, weldments allow another technique that might meet your needs.

In the drawing, place a view of the assembly. On the Model State tab, pick Assembly, Machining (shows welds and post weld machining), or Welds (shows welds). Place your parts list based on a view of the assembly.

On other sheets, place a base view, and from the same selection tool, drop down the Preparation list. Each component in the assembly is listed there. Pick the one you want to detail, and place a base view and any other views of the part as required. Repeat 50x (or as needed) to get all the parts. Balloons attached to the parts in the "part" views will maintain the link to the parts list since they are technically all views of the same assembly. Each part will also show any pre-weld preparations added at the weldment level.

Neil

[AnchorChain]

Kirk,

It sounds to me that you had the exact same issue that I am having now.  The problem with going to a one part/one drawing system for us is the exponential increase in paper that would be used when we issue drawings to the shop.  Now if our shop had an electronic system in place it wouldn't be an issue.

Thanks for the help,

AC

[blair]

We export all drawing to DWF including the solid 3D model. We have industrial tablets on the shop floor and they can access the DWF's via our W-LAN.

[karthur1]

Point taken about the increase in paper.  We dealt with that too.  However, we went from using 24x36 to 11x17 sheets for the detail parts.  We were also sending some parts out to other shops for manufacturing and the single drawings helped with that.

One problem that we were having with the multiple sheet idws is that they would get really large and take a long time to open/update.  So, rather than putting all the idws in a single file, we would still use only one sheet, but append the name ...sheet1, sheet2, sheet3... etc to the filename. Like,

Job xxxx-101-sheet1.idw

Job xxxx-101-sheet2.idw

Job xxxx-101-Sheet3.idw

In this case, the part number was xxxx-101.

Normally, sheet 1 would be the overall drawing (weldment or assembly) and it has an overall parts list.  When we balloon the parts in the weldments, we would use a split balloon.  The top represents the item number, the bottom half is the sheet number the detail is on. Each part has a custom iproperty named "Sheet_Location" that it gets this information from. Thats easy to do if you have iProp Wizard (its also easy to change later if the part moves to another sheet).

 Sheet 2 thru whatever would be the detail parts.  This made it more managable when the drawings required updating and it keeps the filesize down as well. Having the details on seperate sheets also made it easier when we needed to revise a part. We can have different rev levels on each sheet if need be.

I sent you a private message so look in you message box.

[mpatchus]

We no longer call out parts by an item number.

Parts in our assemblies are ballooned with their stock number.

We then use the stock number in the VIEW ANNOTATION as the title of the detail view.

So our views come out as  DETAIL XXXXX.

Since this is set up in our styles & templates, it is entirely automatic for part details.