Drawing BOM issue

[KulbirSandhu]

Hi

I have some drawing issue regarding manual BOM creation in which I failed to change the order of bom items and their qty. My company needs this format. Please Refer attached drawing pdf for detailed queries.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[RonSt.Pierre]

to change order in your bom, use:

table > repeat region > Fix Index; <select bom>

order as needed (select item number, enter new position number; repeat)

regarding the bom quantity.

Your attributes are set to no duplicates.

When I change them to duplicates, the quantity fills in (reduces the bom in half)

I am not sure so if others know, please chime in, but I believe because you have no duplicates selected, it disables the quantity reporting.

If this be the case, you could write a bom relation like "bom_qty=1", then in your bom column for report parameter "&rpt.rel.bom_qty"

(menu select: < rpt  > rel  > USER DEFINE > <type in "bom_qty">)

Regarding the green lines, these are for sheet metal, it indicates the base side of the metal.

It is a modeling reference.  to remove the color from your pdf, select within the pdf creation menu to create only black and white output

[KulbirSandhu]

Dear Ron St.Pierre

You almost solved the problem. The updated drawing is in the attachments. Now new situation is that attributes with no duplicates also merged the mirror components, however component 1 has its two variants (original & mirror). In solidworks components configuration remains different for bom, but here i used flexible tool to configure mirror components. If i use create part by mirror in assembly then changes made in original, will not reflect in mirror component. How can this be resolved?

By the way thanks.

Kulbir Sandhu

[RonSt.Pierre]

Just playing around...

personally, I do not like to have suppressed features in a part unless they are part of a family table.

I removed the flex from the bottom ch1 (in model tree), then saved a new part as ch1a and did a replace of ch1 with ch1a

I removed the flex from the top ch1 then removed the suppressed features (mirror and solidify)

Net effect:

you have a right and left hand item 1 and 2.  this did not effect your drawing.

In the bom outside the drawing frame, I added a column with a report parameter of "&asm.mbr.name" and a column with "&rpt.qty".

I changed the repeat region attribute to no duplicates and all fields populate now. (description, mass, qty, name) with 4 items being reported
In my mind (which is usually out in left field) is how this assembly should be built.

When switching back the repeat region attribute to duplicates, the qty column does not populate and I now have 6 items so it seems it will not report qty when duplicates is selected.

What it's coming down to is what items you are reporting in your bom is to how it is going to report.  the more variation, the further the segregation of items.

[KulbirSandhu]

This means that system is unable to differentiate two flexible components however its flexibility changes the whole geometry by length and profile and will show as one unit.

[RonSt.Pierre]

Kulbir,

At this point, I am at a loss like you.  Perhaps some one else can shed some light on this topic with regards to flexible components in BOM reports.

Good luck