Editting standard for hole call outs (".112in" as opposed to "4-4

[aetherTap]

Hey everybody, let's see if I can stump you with this one.

Recently the company has been migrating to Inventor 11 and the manner in which we create BOMs is a bit complicated because the way we call out standard holes is in conflict with the ANSI automation used in Inventor.

If I have a hole in my part, made by Inventor to be a 4-40 screw size, but I want the drawings to show the decimal representation automatically, is there a toggle or option of some kind to change the standard? There are people in the company that refuse to change the company's standard procedure and are taking the point of view that "we shouldn't have to change just because Inventor says '4-40' instead of '.112' ".

Any help here? The two extreme options are to use Inventor's standard or to manually change what inventor gives and lose the ability for the hole callouts in the drawing to be linked to the model changes.


Thanks guys, I would think maybe some other people have run into this?

 

[btrueblood]

Um. 4-40 is a correct terminology for inch size screw threads, per ANSI B18. Calling out standard threads (wire gage numbers 0 thru 12) by a decimal size is flat wrong; if you ever send a print out for work, all bets are off as to what you will get.

 

[aetherTap]

Unfortunately, I am not in a position to change peoples' minds on this issue as of right now. Ha

The real question is whether I can get best of both worlds; appease them by using the decimal representation, but retain the functionality of Inventor...

Any ideas?

 

[powerhound]

I agree with btrueblood wholeheartedly. Keep in mind that Inventor doesn't say 4-40, ANSI does. It isn't Inventor's standard, it's ANSI's. If your company wants to work outside of established industry standards they are just asking for trouble at some point.

Powerhound
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Inventor 11
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[aardvarkdw]

bpmirsch,

Before I explain to you how to do this, I want to chime in with everyone else and say DO NOT DO THIS! This is a huge mistake on your part and on your engineering manager's part for not stepping up and correcting this NOW. Do not perpetuate bad practices just because "that is how we always have done it" or other similar arguments. Wrong is wrong no matter how you justify this and if you sent me a drawing that claimed to adhere to ASME standards and I saw that as a thread callout, you would get at the very least a phone call asking you to explain where you got your information because that is not a proper thread designation. If you don't speak up about this now and get the ball rolling it may never be fixed.

Okay, rant over. Browse in Windows Explorer to program files\Autodesk\Inventor11\Design Data (or wherever your installed the program), and look for a file called Thread.xls. This is the thread tables for inventor. Open the file in Excel and in columns "B" and "C", change the thread designation to read how you would like to see it. Save the file and then open or restart Inventor. You can copy this thread table to everyone's computers so that you only need to make the change once.

A word of caution, do not change the format of the table, you will not like the results. Furthermore Before beginning, save an unaltered copy of the spreadsheet somewhere safe just in case.

I want to reiterate that I do NOT in anyway guarantee this to work properly for you (so be sure to save that copy), and that I do NOT in anyway recommend this as a solution for bad drafting practices. I am providing this to you in answer to your hypothetical question of whether or not you can change the thread callout format, not as a means of circumventing the established standards in order to appease some stick in the mud engineers that refuse to do things so that EVERYONE, not just themselves, can understand.

David

 

[aetherTap]

aardvarkdw,

Thank you very much for the info there. Sounds like an interesting idea and I will be investigating it.

Everyone,

You have to understand that I feel the same way as you all do. I, however, am not in the position to demand changes. I can only offer suggestions as to how things could be. This issue has been brought up before and I guess some people like to adhere to selective editions of standards. haha

 

[BOPman]

Just to add my $.02, the tabs at the bottom of the spreadsheet are the thread types you choose from in your pull-down within the 'Thread' command. If you wanted to create a new thread type all you would need to do is create a new worksheet and name it accordingly. Still, the new worksheet would have to match the existing formats EXACTLY. For example, we use Gagemaker to create ANY size and standard form of thread. I created the worksheet in Thread.xls and named it 'Gagemaker.' Everytime I run a new thread size I enter it into the spreadsheet and it appears in the pull-down.

Also, anytime you modify the Thread.xls spreadsheet, you HAVE to restart Inventor so it'll reload it. If you notice, Inventor only loads the spreadsheet the first time you use the command.

 

[aetherTap]

BOPman,

Yeh that was the approach I was thinking about doing. Seems cleaner that way.



Turns out that I am going about this the wrong way... The problem is not necessarily calling out the holes on the parts that received a bolt, washer, etc. The problem is that the 3D content available for use from the Inventor parts databases are in accordance with the standard and there does not seems to be a way to make the reference to such a part use the ".112-40" instead of "4-40".

This has to do moreso with parts lists than it does with hole callouts in drawings.

Now, of course, this is probably the same 'ethical' problem as talked about earlier, but it is slightly different in terms of how to go about circumventing it.

Any new ideas?

 

[aardvarkdw]

Why not just create your own parts and give them whatever description you want? Our company has part numbers and descriptions for all of our fasteners and therefore we cannot use the Inventor parts for the same reasons you have. Also I don't like the models that they have in the inventor libraries, I prefer to model things myself and then I know that they match the parts we get from our vendors.

Another approach I just thought of is, why not just save the parts inventor database and then save it as something else and change the iproperties? This will change the description in the parts list without having to edit any spreadsheets or databases.

David

 

[BOPman]

If the model is to your like-ing, then cut and paste the model to a new location (i.e. 'My Documents'.) Open the new saved model, and you can then change anything about it including the iproperties.

So long as the model is not saved in a folder that contains the word "library" in it, you can alter anything about it. You could then change the callout for a thread to read differently as stated earlier.

The "Content Center" is going to read the same 'Thread.xls' spreadsheet. If you modify it to read '.112-40' instead of '#4-40' you could then modify the thread feature to read what you want.

After you have the model modified to what you want, you can then cut and paste it back in the directory it was originally removed from.

 

[btrueblood]

Geez, how do your purchasing people order nuts, bolts and screws?