Quantities and Units of Measure in Virtual Parts

[Anonymous]

I've been looking through the various helps files an donlline articles on the subject of virtual parts and I really haven't come across a clear cut procedure for adding quantities to Virtual Parts.

We're using Inventor 2013 and thatnks to teh help I got here, I was able to add the virtual parts with ease. However, I need to add a quantity and a unit to these parts so that they show up in teh BOM correctly.

For example I have the following virtual part

p/n: 1000009320

Qty: 100 FT

Decription: CABLE, 14AWG, 600V, FOIL SHIELD, 4 COND

As I said, adding this was easy. But now a quantity of "1" shows in the BOM and need 1000Ft to show up.

When I worked with Solid Edge I was able to right click and access their version of iProperties and add the quantity as well as the units. But when I look in the iPropoerties for this virtual part I don't see anywhere to do this. I can manually change the quantity in the BOM but that seems like wrong.

I also know that you can right click on the part in the tree and select "Component Settings" and change the Default BOM Structure for that item. And there is a "Unit Quantity" box but it looks like it's read only (even with the main assembly checked out)

Am I missing something here? This seems like it should be an easy operation

[mdavis22569]

Is it a 1000ft?   

If it's a length you want, then you'll need to populate the BOM with that value/parameter... 

It'd be much easier if you attach an IPT/IDW to show

[SBix26]

In 2016, at least, right click on your virtual component in the assembly browser and select Component Settings...  This presents the units and quantity settings.

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

[Anonymous]

No, it's 100 FT.

This seems like a pretty simple question so I'm not sure how me uploading a IPT or IDW file would help. You can easily make a Virtual part with the parameters I described in my original post and drop it into an assembly, then make a drawing.

I'm positive you will see the same thing that I have since I have had several people at work do the same thing.

There should be an easy way that you define a quantity and unit for a virtual part. How else would you show something like "20 oz of Hydraulic Oil". You can easily make the virtual part called "hydraulic oil" but how do you specify "20 oz"? I find it really hard to believe that the Programmers and Techs at AutoDesk didn't make adding Quantity and Unit to a virtual part an easy process.

While I was typing out the response above I had a chance to look over the IDW and try something else. I right clicked on the BOM and then selected "Edit Parts List" from here I was able to manually type in "100" in the QTY column and "FT" in the UOM column. And it seemed to work. While it still seems a bit too "manual" for me, I can see why this may be the process for making it so that qty and uom are shown in the BOM for a virtual part.

Is this the prescribed method? It seems like it woul dbe more logical that there would be an iProperty for Qty and UOM in the Virtual part

[Anonymous]

Sam,

If you look in my original post you'll see that I reference the dialog box you have shown

What I have found is that that I cannot change the Unit Quantity. It acts like it is read only. And the Base Quantity drop down just reveals a listing of the parameters.I find it kinda' hard to believe that I would need to make a new parameter in the assembly just to use as a unit of measure for a virtual part. That's the kind of information that should be inherent to the virtual part itself.

I have a feeling that we are approaching the answer to this question and it's just a matter of checking a box or accessing a hidden property.

Thanks for your input.

[swalton]

I don't use virtual components.  Instead, I use an ipt file without any geometry.  That way, I can use that ipt in other assemblies, without re-entering the data.

Here is my method for wire in 100 ft spools:

1. Create a new ipt
2. Create a user parameter that counts the purchased length
3. Edit the bom settings in the Tools|Document Settings window.
4. Change the unit of measure to my new user prop.
5. Edit the iprops for description, part number, vendor, vendor part number, etc.
6. Place the wire ipt in an assembly. 
7. Use "Ground and Root Component" from the Assembly|Productivity fly-out to lock the wire part in place
8. Create a component pattern with a 1" offset and the proper number of occurrences that I need for the assembly.

I have attached an example in IV 2014 format. 

[swalton]

I just re--read your post and saw you are on IV 2013.  Here are some screenshots of my process.

Part User Parameters:

Part Document Settings:

Part iProps:

Assembly Structure and BOM

Part List on an IDW

I edited the QTY column for units and precision.

[Anonymous]

Unfortunately I cannot open the example you provided since it is a later version of Inventor. But I understand your methodology perfectly. Honestly, your solution makes MUCH more sense than using the Virtual Parts. This way you can actually save them to Vault and have them be administered through that program.

If I understand correctly, in the IPT itself you make a User Parameter called "Purchased_Length" and give it a value of "100 FT"

After that you refer to that user parameter in the "Bill of Materials" tab of the iProperties. But, once again, I think that feature may not be in my version of Inventor (2013). I just looked at an IPT and checked. There is no "Bill of Materials" tab

So I think we are back to square one.

[swalton]

The BOM tab is not in the Iprops window.

It is in the Document Settings window.

See the link below for the IV 2013 online help page about Document Settings.

http://help.autodesk.com/view/INVNTOR/2013/ENU/?caas=caas/vhelp/help-dev-autodesk-com/v/Inventor/enu...

[SBix26]

Sorry, there's no image in your original post, at least not in my browser.

I am able to set the base unit to Ft on a virtual component, but if I set it back to Each, then it's grayed out and changes to match whatever parameter you choose.

I don't see the big deal about the parameters, though.  The quantity needs to be stored somewhere, I guess, and parameters can calculate from each other, so it might have benefits.

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

[Anonymous]

Ok, I got it now.

However, I have a question regarding the re-use of this IPT file in a futire assembly that requires a different length.

In the IPT file there is this user parameter and it's set to 100 ft. So I want to use it in another assembly but I need 25 feet. So in order to not screw with my previous assembly I need to copy the design of the old IPT and name it something distinct.

Correct?

[Anonymous]

I've been experimenting with the use of pure virtual parts as opposed to using an indivual IPT and I think I might be on the right track (that remains to be seen)

The steps are

1.) make the virtual part in the assembly as previously detailed

2.) set up a User Parameter in the assembly that details the quantity and unit

3.) right click on the virtual part in the tree and select "component settings"

4.) Under Base Quantity, select the appropriate User Parameter

5.) Check the BOM and se that it shows up

So far I can get the quantity and units to show in the BOM. However, I have been having difficulties getting the quantity to show in the IDW's BOM. And this appears to be a setting in the Parts Lists that myself and another employee need to investigate.

One thing I was wondering is what do you do when you have a virtual part and you need 100 of them. But there are no units involved. Like 100 wire ties. You can't make a user parameter that says "ea". The closest one is "Unitless" ul. And when you do that it will not appear in the list when you go to select "Component Settings"---> "Base Quantity"

Any help here?

[swalton]

I see 4 options:

1. Copy-design to a new file and adjust the user parameter, as you discussed.
2. Change the user parameter to the shortest length you will ever use, maybe .25 ft, and increase the pattern count in the assembly to get the correct total length.  This way you don't have to make a new part for each assembly.
3. Convert the wire part to an ipart and publish it to the Content Center.  Set it up so that the length user parameter is a variable, like the structural steel sections.  When you add it to an assembly, place it "as custom" and adjust the length and assign the filename then.  You could add several rows for each type of wire that you use, maybe by AWG or color, etc.  
4. Like option 2, but make the wire part into an ipart to capture all the different wire specs you use.

[SBix26]

I can't see any choice but to place 100 of those virtual wire ties.  This looks like an improvement that should be made in Inventor.  Work up a proposal and put it in the Inventor IdeaStation forum, then post the link back here.  I'll definitely vote for it.

Sam B

Inventor Professional 2016 Update 2
Vault Basic 2016
Windows 7 Enterprise 64-bit, SP1

[Anonymous]

Ok, I submitted it as an Idea

http://forums.autodesk.com/t5/inventor-ideastation/add-iproperties-quot-quantity-quot-and-quot-units...

[Anonymous]

I've been trying to dial this in:

Would really prefer for the Unit QTY to read "ft" and the QTY to read "20".  Is there a way to do this that I've missed?

Inventor 2020.1

[johnsonshiue]

Hi Larry,

It is doable. You will need a parameter at the assembly level. Create a LENGTH parameter in ft unit in the assembly. Right-click on the virtual component -> Component Settings -> select the parameter as Base Quantity. It will show up as such on the BOM table.

Many thanks!

[Anonymous]

Thank you for taking the time to respond Johnsonshiue, it is greatly appreciated.

Your approach is pretty close to what I had been trying.  You did get me closer than I was before:

I was hoping for a Unit QTY of "ft" instead of "1.000 ft" but this is much better than I had before.

One step I'm going to add in case someone else is trying to accomplish this is:  At the end of the procedure you suggested, in the Bill Of Materials, I right clicked in the QTY field and changed from "Calculate Quantity" to "Static Quantity".  This allowed me to enter the 20 ft in the QTY field.  

Thanks again for your help.

[johnsonshiue]

Hi! This depends on the display precision and the input value. You can go to Tools -> Doc Settings -> Units -> set the Displace Precision to no decimal paces.

Many thanks!

[majnalt]

pattern the virtual component