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Content Center / Parts Lists Frustrations

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Message 1 of 11
Mark.Hopkins
3033 Views, 10 Replies

Content Center / Parts Lists Frustrations

Can anyone help me please.

 

Im trying to customise my parts lists so i never have to manually edit anything.

 

I'm having trouble formating units.

I have assemblies made up of parts with mixed units - i.e pipes in imperial measurements and some members in metric units. This cannot be helped

 

I want to show all measurements (lengths) on my parts lists in metric.

With a precision of 0.

 

I want to show in the unit qty field "Each" where the measurement is by number of items, parts etc.

 

Does anyone have any guides or help on this subject?

 

10 REPLIES 10
Message 2 of 11
pauldoubet
in reply to: Mark.Hopkins

Mark,

 

Please remember to include the version of Inventor you are using.

 

"I want to show in the unit qty field "Each" where the measurement is by number of items, parts etc."

 

This is not required and actually should not be changed. If you look at the Help for Inventor you will see that Inventor provides several Qty properties for use in the BOM data and resulting Parts Lists. All that you need to do is use the 'Item Qty' property in your parts list and you will never have to change a 'Unit Qty' in most cases.

 

Please provide your version of Inventor and I or someone else will help you with the formatting.

 

Paul

Message 3 of 11
Mark.Hopkins
in reply to: Mark.Hopkins

Ah sorry, I have inventor suite 2011
Message 4 of 11
pauldoubet
in reply to: Mark.Hopkins

If you could explain your mixed units it would be helpful in providing a solution. Are the pipes coming from Content Center, are the other parts coming from Content Center or are they being created from your template file? Do you understand using the export parameters and formatting the exported parameters?

 

Paul

Message 5 of 11
Mark.Hopkins
in reply to: Mark.Hopkins

1586iB589A027302BE225 

 

You can see my problems.

The last line has a piece of astm pipe in imperial measurements

 

When I insert a part from content centre or from frame generated parts, the length on the parts list will either be in mm or in inches, depending on which standard it is from.

I need all lengths in mm with the precision to either 0.00 or 0.

Frame generated parts always have a precision of 0.000

 

I have tried formating to mm in the parts list style of the unit qty and qty fields but i get a lot of incompatible units errors.

For individual parts, I need the unit qty to be "Ea" or "Each"

 

No im not sure what you mean by exporting paramaters but willing to give it a go

 

 

Message 6 of 11
pauldoubet
in reply to: Mark.Hopkins

I am going to be doing some guess work here because I don't know exactly what you are doing with all the blue boxes showing in the parts list, except you are doing alot of overrides to existing BOM data. In other words I know why the blue boxes are there, I just don't understand why you are doing the overrides.

 

I may have to post more than one reply to get the attachments uploaded. Also it usually works best to post a screen capture as an attachment in png or jpg format instead of embedding them.

 

In the attachment 'Parameters-Unit Type' you can see the parameters page for the same CC part you have on the last line of your screen capture. Please note that I actually changed the units to mm on the B_L parameter, this is incorrect, I should have changed it on the G_L parameter. B_L stands for Basic Length and G_L stands for Geometric Length, the G_L is the length that would be correct if you trimmed a CC part with Frame Generator.

 

You access the parameters page from the Manage tab, then the Fx icon. Then you highlight the G_L parameter and change the units to mm and check the Export Parameter button as shown in the attachment 'Parmeters-Custom Property Format'. Then you set the Precision and change the Units String, Leading Zeros, and Trailing Zeros to meet your needs.

 

Then you open the BOM editor and select the 'Add Custom iProperty Columns' near the top of the dialog box. Click and type in the G_L, then click the OK button. I have shown the resulting column added to the BOM data in the attachment 'BOM with Custom iProperty'.

 

I have also attached a PDF file (to the next reply) that should be helpful in creating a Custom Content Center and formatting the iProperties to meet your company needs.

 

Good Luck, Paul

Message 7 of 11
pauldoubet
in reply to: Mark.Hopkins

Here is the PDF file.

 

Paul

Message 8 of 11
Mark.Hopkins
in reply to: Mark.Hopkins

Many thanks, the battle is half over.

I havnt any training on configuring content centre so your PDF was really very excellent thanks.

I have another couple of questions which may solve the remainder of my problems.

 

Found that in some content centre items, the G_L is actually the PL parameter.

 

Which means many items will have no value on the BOM custom iproperty field

 

In this field, can you use a formula something like you can in a spreadsheet?

 

Something like -

 

"If there is no value of G_L, then use PL, if there is no value of PL, then use the text "Each" 

If it can be done, can you provide the syntax?

This would then cover all options that I require in this field.

 

Are we heading into Macro territory?

 

The only drawback is I still have to manually edit the unit of the G_L or PL paramater on every imperial part - each time?

At least this is a lot more preferable, than manually over riding the value on the parts list

 

Can I change the units of the family table?

 

Or creating my own parts and publishing to the content centre, which could be very time consuming initially.

 

Any help is appreciated.

Message 9 of 11
pauldoubet
in reply to: Mark.Hopkins

Your PL parameter is present in your CC part because the part originated from the Tube and Pipe CC category, the one I used originated from the Structural Shapes category. You may use either, I would recommend that you decide which one to use and stay with that category & family since your end goal will be much easier to achieve if you always use the same one.

 

Through a combination of the 'Rollup on Part Number match' in the BOM editor and the 'Group' function in the Parts List you can usually achieve what you want. The other option is to use Custom iProperties which allow you to define each type of part with a unique formula that equals a particular parameter or iProperty.

 

If you setup a Custom Content Center you can change the units in a part file created from that CC family and then use the 'Replace Family Template' function to make all part created by that family have the length units = mm. Creating your own CC for something like the imperial pipe sizes takes less than five minutes once you understand what steps to follow and what to change. As an example of how easily iParts, iAssemblies, and Content Center parts can be created I have created in excess of 30,000 parts/assemblies in the last 3 months. Once you take the time to study how these parts work and how to change part sizes and arrangements this is a very powerful and useful tool.

 

Paul

Message 10 of 11
Mark.Hopkins
in reply to: Mark.Hopkins

Many thanks, Almost there.

 

Have edited the custom cc family table,  and changed all sizes and descriptions, units etc to mm.

Then edited a part file generated from this table, changed the units in doccument settings of the sketch to mm, changed all paramaters of the part to mm, and used the part to replace family template.

 

When I then generate a new part file, All measurements are in inches (ie a 168mm OD pipe will be generated as 168 inches) Paramaters of thet newly generated part revert back to inches. 

 

Is there a units setting i need to change elsewhere?

Message 11 of 11
pauldoubet
in reply to: Mark.Hopkins

OOPS!

 

The only thing you should have changed was the PL or G_L parameter if I understood what you wanted to accomplish. I thought you needed to use imperial pipe sizes with the cut length in mm. If so delete the family table and start over or go back and change everything back to inches except the PL or G_L parameter.

 

Good Luck, Paul

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