Part numbering options

[Andy330hp]

I made mention of this in my other thread, but since it was off topic I'm starting a new one

I've noticed that Solidworks has more than a few different points within a drawing where you can enter a "part number". One is custom properties, one is configuration specific properties. You can also enter in part numbers in the summary title field, the configuration name, and the file name. There may even be more, I feel like every time I open a different window there's another opportunity to enter a part number that may or may not have any significance to anything else. For some reason, at least in my experience, I have been able to to point the BOM part number reference to the last three via a pulldown menu in the configuration properties, but not to the first two (which is unfortunate becuase I spent the last day filling in those fields for for 50+ files becuase I thought I was doing it right. Ouch!). Where in your files do you assign Part numbers, other than in the file name, or do you not even bother?

 

[TheTick]

We assign part numbers in the custom properties, and have the model p/n carry through to the drawing.

I will be expanding our part-numbering format to incude pre-release and released part numbers.

I'm not hung up on any paricular method. We do what works best for our current documentation and PDM situation.

All this machinery making modern music can still be open-hearted.

 

[Andy330hp]

Has anybody had problems with part numbers assigned to toolbox items not showing up in the BOM?

 

[Andy330hp]

I take that back, now all my part are having the same problem: The file name is being used instead of the custom properties field in my BOMs. What did I change?

 

[Standing]

Andy330hp,
Check in your bomtemp.xls to see what the “Named Box” is, when you highlight row one of the part number column. Now see if the “Named Box” is the same as the custom Property, is the same as one of your parts. If I understand what you are asking this should be the same and fix it.

Bradley

 

[StarrRider]

Andy330Hp

I will try to explain but I am using SW2001+ so there may be variations between what I see and what you see OK.

SW used the existing File Properties format that MS created and built the system so that the user could customize it in any way they saw fit. This allows you to create/modify the File Properties and Custom Properties (everything except Configuration Specific Custom Properties) in other programs like Windows Explorer.

How you set your system up to work depends on you, but by default, when you open the File Properties Dialog / in the Summary tab there are 5 edit boxes named Author, Keywords, Comments, Title, & Subject. The Title field is used to contain the Part Number on most systems. For this to function, when the Bill of Materials is added the check box “Use summary information title as part number” must be checked. If it is not checked – then SW looks to see if there is a Custom Property named “PartNumber” and uses it or the file name if it isn’t there.

The other fields on the Summary tab are not used as frequently. I use a macro that places my name in Author field. I also use the Subject field to contain the Product and the Keywords field to contain the major assembly that the model will be used in (Pneumatics / Electrical / Options / whatever). I also place the creation date in the Comments field unless the part is a Purchased Item and then I put the Vendors Contact Information with their part number in there.

The Custom and Configuration Specific tabs are nearly identical. The only difference is that a Custom Property applies to every configuration except those that have a Configuration Specific Property with the same name. – So – If you created a part with a CP named “Dog” / value = “Mongrel” and then add a Terrier Configurations and use a Configuration Specific CP named “Dog” / value = “Terrier”. Then – In the assembly drawings BOM (created to use the CP), every instance of your part would report “Mongrel” except the Terrier Configurations, which would report “Terrier”.

Actually - There are a few more twists and turns than that. SW also gave the BOM a little intelligence. It allows the BOM to look at the Part Number and Description and join them together when they were identical even if they were different parts. An example is needed to explain this – So - Lets say you have a wiring harness used on an assembly and you need to show where it is hooked up and how it is routed. The harness has 3 different kinds of connectors so you create a model for each one with a tail to indicate direction the wire should go. You insert each of these connectors where needed. You also create another part that sort of looks like a bunch of wires twisted around each other and you insert it in various places to show the routing of the harness. In the drawing, you create detail views each of these connections and call them out with a balloon. Your isometric view shows the routing of the harness with additional balloons. Problem – the balloons report different item numbers and your BOM has 4 parts with different quantities where there should only be 1 Wiring Harness.

So how do you handle this? You could shove all of these parts into another assembly to get everything to report correctly in the BOM - But then if you moved any of the related parts that assembly would need to be repaired – further you would have to create a bunch of configurations or hide a lot of parts so that your detail views worked properly. Fortunately – if all of these parts have the same Part Number and Description then SW will consider them the same part in the BOM. The quantities will still be wrong but your system should allow you to override that and display the quantity that you need. The only problem left is the balloon numbers – they are reported correctly in the view that has the BOM attached but are wrong everywhere else (SW99 & SW2000 did this correctly but there was a change in SW2001 after a couple of SP which caused errors - SW2001+ had the same problem – I do not know what SW2003 does). To get the balloons to be correct – add a BOM to each view and hide it.

I hope this helps.

Lee

Consciousness: That annoying time between naps.

 

[mushin]

Hi Andy:
I ran into this recently when I modified a toolbox part and renamed it to a formal part number. I started with a piece of structural steel channel which kept showing up as a C8 X 13.75 in the BOM. I could not get it to change to the drawing number even though it showed up correctly numbered on the drawing detail.

What you have to do is, open the part file and go to the configuration tab. If you right click on the default configuration, a box appears. At the bottom is a small window that shows you what appears on the BOM. Below it is a drop down menu that gives you a choice of picking the document name. Once you do this, the BOM will update with the correct part number.

 

[Andy330hp]

I looked at my BOM, and it's cell name was partno, not PartNumber as StarrRider suggested, so maybe that's my problem? The thing is, my custom property is partno, so it should work. Actually, it's PartNo, is the BOM case sensitive? I may also just try renaming both to PartNumber and see what happens....

 

[TheTick]

Accessing custom properties is case sensitive.

All this machinery making modern music can still be open-hearted.

 

[Andy330hp]

dang it....

 

[TheTick]

Actually, it is case sensitive when being accessed. However, you can not have multiple properties differentiated by case, such as "name" and "Name".