Thread specification as parameter

[Anonymous]

Hello

I am wondering if it is possible to control thread specifications by parameters so that I can change a lot thread features by just changing one parameter.

Thank you

Daniel (Inventor 2016)

[bobvdd]

Attached is a 2016 part file that contains an iLogic rule that reacts to the value of a single Inventor parameter called "Threadedholesize".

The iLogic rule scans through ALL hole features in your part and changes all of them.

You can change the value of the "Threadedholesize" parameter either in the parameters dialog or through the iLogic form that sits in this file.

I used a couple of ANSI Unified Screw thread sizes as example.

IMPORTANT:  when you create holes with the linear placement, make sure that the references to edge 1 and edge 2 are defined, otherwise the rule won't work.

Dim Myarraylist  As New ArrayList
Myarraylist.Add("3/4-32 UN")
Myarraylist.Add("1-32 UN")
Myarraylist.Add("2-6 UN")
Myarraylist.Add("3-8 UN")
Myarraylist.Add("4-6 UN")

MultiValue.List("Threadedholesize")= Myarraylist 

Dim opartDoc As PartDocument
opartDoc = ThisApplication.ActiveDocument
Dim oHoleTapInfo As HoleTapInfo
oHoleTapInfo = opartDoc.ComponentDefinition.Features.HoleFeatures.CreateTapInfo(True, "ANSI Unified Screw Threads", Threadedholesize, "2B", True)
Dim ohole As HoleFeature
For Each ohole In opartDoc.ComponentDefinition.Features.HoleFeatures
  ohole.TapInfo = oHoleTapInfo
Next ohole

Here is a screenshot of the iLogic form in action.

[Anonymous]

Thanks, great! I will give it a try.

However, it would be tricky to parameterize two different types of thread. I think it would be a nice feature of Inventor of thread specifications could be defined as parameters in some way.

Thank  you

Daniel

[mcgyvr]

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@Anonymous wrote:

Thanks, great! I will give it a try.

However, it would be tricky to parameterize two different types of thread. I think it would be a nice feature of Inventor of thread specifications could be defined as parameters in some way.

Thank  you

Daniel

---

Not sure what you are trying to do but have you looked into creating an ipart?  You can edit the threads in the ipart table/excel fairly quickly

[Anonymous]

Hi,

I am using the workflow of constructing a simple assembly as a part file and then use the 'Make Part' tool to derive the individual bodies in this file into an assembly. I have two types of threaded holes, which have undefined diameters/specifications at this early stage of design. So I thought if I could introduce two parameters which control the specs of these two types of threaded holes, that would simplify my setup.

Daniel

[bobvdd]

Another thought. In case you would prefer to choose iLogic over iParts and are dealing with creating multiple part files and don't want to embed the iLogic rule in each of them, think about using an external iLogic rule which you can create once and for all.

Cheers

Bob

[Anonymous]

Like you, I will prefer to have it in parameters.  We already have hole depth in parameters.  We do not and will probably never used ipart or ilogic at my job...