I did a quick experiment to make sure this method would work with tapping existing holes. When I use this method it is typically to do more machine work to the assembly and not tapping holes.
Here is the workflow I used:
1. Create individual part, with drilled holes.
2. Create an assembly from the individual parts.
3. Create a new derived part from the assembly.
4. Use the "thread" command to tap the existing holes.
This method worked, but not as well as I had hoped.
The problem I encountered was that the thread command would not let me select multiple holes at once.
I had to apply the thread to each individual hole, which could be very tedious if you have a large number of holes.
The biggest issue is at the drawing level. Since each hole is threaded individually dimensioning does not recognizes the holes as a group, so you still have to edit the dimension to include the proper quantity.
I had hoped this would be a more elegant solution. I guess this just may be another case where its difficult to recreate in Inventor what actually happens in real life.
Richard in Houston
OK, i'll accept this, I thought I was going crazy when I couldn't find the thread feature, but that is only available in the part level and not assembly level:
Well, if I am going to use this method, I will have to do another test and see if that the BOM/parts list shows the individual parts for assembly on a idw.
At least I can get thread to show up on the final assembly view.
Thanks for now!!!
I don't have much experience with derived parts, but after trying to create a drawing using my example. I can't identify the unique parts that the assembly is comprised of. In the parts list I would like to show what the assembly is made up of and qty's.
So unfortunately, using a derived part will not be a good method for this issue.
The only other option I can think of is to get rid of the holes in the part level and then add the threaded holes to the assembly. If the fabricator wants to laser cut the holes before assembly, I suppose he can take the initiative and figure it out based on the hole centers off the assembly drawing, figure out what the drill size is for 3/8-16 UNC and go from there.
Doesn't seem right, but at least this way, I have a drawing showing final outcome. I don't really care for this particular part how it is made.
Not even sure if I can make a suggestion to the idea station forum for this issue, I know why I can't add threads to the part features inside an assembly. If the part features change, then the threads at the assembly level will result in an error. Example: holes currently in parts is 5/16", which is the drill size for 3/8-16UNC. If changed the holes in the parts to 1/8", Inventor wouldn't know what to do with the 3/8-16UNC holes in the assembly level. The major issue lies with why can't I add new threaded holes in the assembly over top the existing the holes from the parts files??
Simply make a plate with 3/8" tapped holes. Create a flat pattern. Edit the flat pattern and create a sketch. Fill in the holes. Create a 5/16" hole with same centres.
The laser/plasma/oxy/water typically only uses the dxf created from the flat pattern and does not care about the model/assy.
Would this not work for you? (You can even have the holes be parameter driven.)
(This is another reason I would like flat patterns to be able to have the option of holes represented by points just like punches.)
Yea, sorry I did read this earlier when you wrote it and meant to reply back.
This just seems like alonger way around, make a flat pattern for a part that is aleady flat. I like how you can edit the parts in the flat pattern they only affect that view. Once you click back to the folded part view the editing is gone. However, this is more work than needed. I would need to create flat patterns for all three parts, ensure that I have selected the flat patterns in the individual part file drawings for annotating, and then for the assembly drawing I could have the proper final assembly with the threaded holes shown.
But if I keep everything as the way I have it, make the correct part files with proper drilled holes (5/16") and then in the assembly drawing, fudge the one hole note to show 3/8-16UNC, it is much less work and it gets the job done. There is no need to visually show the threads, and the part will be made accurately based on the individual part drawings.
I will keep this in mind though for future issues that can be resolved by this method.
I think the answer to this could lie within the part view representations. If we had more control over part features, then a view rep could be setup in the assembly to show either the blank holes or the threads.
I wonder if this is something Autodesk could fix by adding a Level of Detail to the part view representation tree.
Yea, this would be another possible solutuion, maybe set up a multi-value user parameter that can changes the holes from 5/16" thru to 3/8-16UNC, and set view reps or possibly use iLogic to show thru holes in the part level and then show the tapped holes in the assembly level. Brain is churning again...
haha, thanks for the reply, might be onto something...