Community
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.
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
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.
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
Accepted solution
@Anonymous 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
@Anonymous 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
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
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
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.
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
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.
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
Inventor 2020, In-Cad, Simulation Mechanical
Just insert the picture rather than attaching it as a file
Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.
Delta Tau Chi ΔΤΧ
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.
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.
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.
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.
Forums Links
Can't find what you're looking for? Ask the community or share your knowledge.
Post to forums
