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Message 1 of 19
Anonymous
810 Views, 18 Replies

BOM FUNCTIONS

Hi UG.
Can anyone explain me what these functions in BOM mean?
I am using some of them but a large portion is unknown me.

Regards
Al
18 REPLIES 18
Message 2 of 19
Anonymous
in reply to: Anonymous

Alex,

Do a search in the Mechanical Desktop help on a function like ISBLANK. It will bring up a list of the various functions
and their syntax. This help information is pretty sketchy from Autodesk. However, the use of these functions in Autocad
is very symilar to their use in Excel and VB.

If you need specific help on setting up and using these functions, let me know. I have done quite a bit of customization
to my BOM's using these functions. For example, I have the size of my parts (XX x YY x ZZ) automatically and
parametrically entered into my BOM for 95% of the details I do. This saves a lot of time and eliminates a lot of error
on my cut-lists. I also have the part number and description parsed automatically (and again parametrically) from the
filename. A great thing about all this automation is if I open a part file, do a save as, and then change the length of
the part for example, the BOM/parts-list are completely updated and correct for the new part. There are many other
things you can do with these functions of course.

Bob W.


Alex wrote:
> Hi UG.
> Can anyone explain me what these functions in BOM mean?
> I am using some of them but a large portion is unknown me.
>
> Regards
> Al
>
>
> ------------------------------------------------------------------------
>


--
Bob Wiley
Mechanical Designer
Swedish Match North America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 3 of 19
Anonymous
in reply to: Anonymous

Bob, I would really like to see one of your BOMs with the formulas. I
struggle through these alot myself sometimes. The syntax seems to be picky
from one to the next and the documentation, like you said, is not very
complete or user friendly. What's entered into one, doesn't always work
using the same syntax in the next.
Message 4 of 19
Anonymous
in reply to: Anonymous


Thanks Bob.

It was very helpful.

I'll play with these.

I am using formula:

=TEXT((SIZE_IN/12)*QTY,".000")

It converts IN to FT, and gives me a 0.123
(it's sample) value with a leading "0"

I want to take out a leading 
"0".

Regards

Al

 

"Bob Wiley" <wile2162removeB4atbellsouth.net>
wrote in message

face=Arial size=2>news:5270524@discussion.autodesk.com

face=Arial size=2>...
Alex,

Do a
search in the Mechanical Desktop help on a function like ISBLANK. It will bring
up a list of the various functions
and their syntax. This help information
is pretty sketchy from Autodesk. However, the use of these functions in Autocad

is very symilar to their use in Excel and VB.

If you need specific
help on setting up and using these functions, let me know. I have done quite a
bit of customization
to my BOM's using these functions. For example, I have
the size of my parts (XX x YY x ZZ) automatically and
parametrically entered
into my BOM for 95% of the details I do. This saves a lot of time and eliminates
a lot of error
on my cut-lists. I also have the part number and description
parsed automatically (and again parametrically) from the
filename. A great
thing about all this automation is if I open a part file, do a save as, and then
change the length of
the part for example, the BOM/parts-list are completely
updated and correct for the new part. There are many other
things you can do
with these functions of course.

Bob W.


Alex wrote:
> Hi
UG.
> Can anyone explain me what these functions in BOM mean?
> I am
using some of them but a large portion is unknown me.
>
>
Regards
> Al
>
>
>
------------------------------------------------------------------------
>



--
Bob Wiley
Mechanical Designer
Swedish Match North
America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell
Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver
version 81.72
Message 5 of 19
Anonymous
in reply to: Anonymous

1 question for multi bom & multi balloon
in multi layout.
Message 6 of 19
Anonymous
in reply to: Anonymous

Alex and Jason,

Take a look at this drawing it has the BOM functions I regularly use in addition to some that will do what Alex is
looking for.

Open this file and take a look at the BOM (AMBOM). Go all the way over to the right most 3 columns and you will see how
I would format the size to drop the leading zero. The first of the three columns has the source size (1.476). The second
has the unformatted calculated size in feet (ES) using the formula you provided. The third has the calculated size with
the leading zero dropped. If you look at the formula in the third column, you will see that the unformatted size (ES) is
referenced 3 times. If I had not placed the unformatted size in its own column then the formula in the third column
would have been VERY long and hard to read.

Now take a look at the column labeled "Size". It is fairly lengthy but is takes the X, Y, and Z dimensions for a
rectangular part, sorts them, and puts them in my BOM. For this to work, My base extrusion must be a rectangle with
constraints d0 and d1 as the length and width. When I extrude the rectangle, d2 is the draft angle which I ignore in the
BOM. d3 is the extrusion distance. So it is d0, d1 and d3 that I sort and use. This works for most all of my parts.
Anything that is not a rectangle to begin with requires me to manually type in the cut size on the BOM. The formula in
this column is not locked so all I have to do is just type over the calculated cut size if needed.

Look at the columns labeled "First space location" (SP), "PARSE" and "Description length" (US). These formulas set up to
parse out the part number and description from the part name (File name). We add an "_S" on the end of all our 3D solid
MDT files to distinquish them from regular Autocad 2D files. This "_S" is trimmed from the file name for the
description. The formulas in columns labeled "Dwg/Part No." and "Description" use the formulas SP, PARSE and US to
actually parse the part number and description. Normally I would have the SP, PARSE and US columns hidden but they are
visible in this case just for discussions sake.

The attached file is "SM-102002 CRANK GUARD COVER_S.dwg" The part number would be all the characters to the left of the
first space. The description would be all of the remainder with the _S stripped away. I can't remember the last time I
actually typed in a part number and description for a part. This works well!

To make all these formulas easy to use requires they be inserted automatically. You don't want to have to type these in
manually every time you need to use them. For some reason custom BOM standards cannot be put in your template file. What
I have done instead is place them in a seperate file that can be inserted as a block into the current drawing. My BOM
standard is in a file called SMNA_std_rev_B.dwg. I then have a toolbar button that fires the macro:

^C^C-insert "S:/TWOLF/DRAWINGS/LIBRARY/SMNA/TITLE/SMNA_std_rev_B" r 0 s 1 0,0,0;_amsymstd

This inserts the drawing containing the BOM standard and runs AMSYMSTD so I can pick a specific BOM standard with it's
associated formulas. I have three standards I use. One for parts, one for assemblies and one for purchased parts. These
BOM standards also set up which columns show up on the parts list that is placed on the drawing.

I have been using these BOM standards and formulas for probably 8 years now. Obviously I did not do all this overnight
and it has required some tweaking. The result has been untold hours saved and errors prevented.

--
Bob Wiley
Mechanical Designer
Swedish Match North America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 7 of 19
Anonymous
in reply to: Anonymous

Thanks, Bob for the great explanations. I'll be able to use some of this in
my BOMs. I didn't know about AMSYMSTD and I'm still not sure how to get it
to work as you described. Had no clue this existed. I couldn't find ANYTHING
in help file on it.

Looking at all the automation in the boms you have, I'm surprised you
haven't taken advantage of fields in your title blocks.
Message 8 of 19
Anonymous
in reply to: Anonymous

Jason,

I have looked into this in depth. I can't figure out how to format and parse the information available in the fields. If
I could link my BOM info back into the fields it would be a no brainer but that does not seem possible. The best I have
been able to do is a VB script that retrieves field information, formats it, and then pushes it into the title block.
That's not a bad solution but I havn't spent enough time on it to get all the bugs out yet. Any ideas?

Bob


Jason Rhymes wrote:
> Thanks, Bob for the great explanations. I'll be able to use some of this in
> my BOMs. I didn't know about AMSYMSTD and I'm still not sure how to get it
> to work as you described. Had no clue this existed. I couldn't find ANYTHING
> in help file on it.
>
> Looking at all the automation in the boms you have, I'm surprised you
> haven't taken advantage of fields in your title blocks.


--
Bob Wiley
Mechanical Designer
Swedish Match North America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 9 of 19
Anonymous
in reply to: Anonymous

It would seem like you could use FIELD and use a diesel string to parcel.
It's been a while since I messed with this but I'll look into it.
Message 10 of 19
Anonymous
in reply to: Anonymous

Well I made you one but didn't realize until after you're using 2006. An of
course it's not easy to do a save as out MDT but I did. You may have to
recover before opening it. It crashed my 2005 here.
Message 11 of 19
Anonymous
in reply to: Anonymous

Jason,

WOW! That gives me more than enough to run with. I have 2007 installed but we have not made a transition to it yet. I
can copy and paste the diesel expression over to 2006. I have never had much need to learn the syntax for diesel. This
will give a reason to spread my wings a little. Looks like my title blocks are going to be automated too.

Much thanks,

Bob W.


Jason Rhymes wrote:
> Well I made you one but didn't realize until after you're using 2006. An of
> course it's not easy to do a save as out MDT but I did. You may have to
> recover before opening it. It crashed my 2005 here.


--
Bob Wiley
Mechanical Designer
Swedish Match North America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 12 of 19
Anonymous
in reply to: Anonymous

I am still at MDT6.0 which I like better than next generations.
I've been using a lot of lisp and some 3 party apps which not working with
next MDT's
but make my life a lot eazier.
MDT6.0 is pretty much debugged and does pretty good job.
I tried 2005 and 2006. They have the same functions as a MDT6.0 exept some
fancy interfaces.
Unfortunately Autodesk ignored parametric surface module in next generation.
So I'll stick to MDT6.0 for a while
If you give me a few screen shots I'll appreciate, since I can not open your
MDT 2006 or 2007.
Regards
Al
"Bob Wiley" wrote in message
news:5271708@discussion.autodesk.com...

Alex and Jason,

Take a look at this drawing it has the BOM functions I regularly use in
addition to some that will do what Alex is
looking for.

Open this file and take a look at the BOM (AMBOM). Go all the way over to
the right most 3 columns and you will see how
I would format the size to drop the leading zero. The first of the three
columns has the source size (1.476). The second
has the unformatted calculated size in feet (ES) using the formula you
provided. The third has
the calculated size with
the leading zero dropped. If you look at the formula in the third column,
you will see that the unformatted size (ES) is
referenced 3 times. If I had not placed the unformatted size in its own
column then the formula in the third column
would have been VERY long and hard to read.

Now take a look at the column labeled "Size". It is fairly lengthy but is
takes the X, Y, and Z dimensions for a
rectangular part, sorts them, and puts them in my BOM. For this
to work, My base extrusion must be a rectangle with
constraints d0 and d1 as the length and width. When I extrude the rectangle,
d2 is the draft angle which I ignore in the
BOM. d3 is the extrusion distance. So it is d0, d1 and d3 that I sort and
use. This works for most all of my parts.
Anything that is not a rectangle to begin with requires me to manually type
in the cut size on the BOM. The formula in
this column is not locked so all I have to do is just type over the calcu
lated cut size if needed.

Look at the columns labeled "First space location" (SP), "PARSE" and
"Description length" (US). These formulas set up to
parse out the part number and description from the part name (File name). We
add an "_S" on the end of all our 3D solid
MDT files to distinquish them from regular Autocad 2D files. This "_S" is
trimmed from the file name for the
description. The formulas in columns labeled "Dwg/Part No." and
"Description" use the formulas SP, PARSE
and US to
actually parse the part number and description. Normally I would have the
SP, PARSE and US columns hidden but they are
visible in this case just for discussions sake.

The attached file is "SM-102002 CRANK GUARD COVER_S.dwg" The part number
would be all the characters to the left of the
first space. The description would be all of the remainder with the _S
stripped away. I can't remember the last time I
actually typed in a part number and description for a part. This
works well!

To make all these formulas easy to use requires they be inserted
automatically. You don't want to have to type these in
manually every time you need to use them. For some reason custom BOM
standards cannot be put in your template file. What
I have done instead is place them in a seperate file that can be inserted as
a block into the current drawing. My BOM
standard is in a file called SMNA_std_rev_B.dwg. I then have a toolbar
button that fires the macro:

^C^C-i
nsert "S:/TWOLF/DRAWINGS/LIBRARY/SMNA/TITLE/SMNA_std_rev_B" r 0 s 1
0,0,0;_amsymstd

This inserts the drawing containing the BOM standard and runs AMSYMSTD so I
can pick a specific BOM standard with it's
associated formulas. I have three standards I use. One for parts, one for
assemblies and one for purchased parts. These
BOM standards also set up which columns show up on the parts list that is
placed on the drawing.

I have been using these BOM standards and formulas for probably
8 years now Obviously I did not do all this overnight
and it has required some tweaking. The result has been untold hours saved
and errors prevented.

--
Bob Wiley
Mechanical Designer
Swedish Match North America

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 13 of 19
Anonymous
in reply to: Anonymous

Alex,

I understand completely about using MDT6. It has not been that long since I was forced to updrade here at work. I still
use MDT6 at home because like you, I find it more stable.

I hope the attached screen shots and spreadsheet will give you what you need.

Bob


Alex wrote:

> I am still at MDT6.0 which I like better than next generations.
> I've been using a lot of lisp and some 3 party apps which not working with
> next MDT's
> but make my life a lot eazier.
> MDT6.0 is pretty much debugged and does pretty good job.
> I tried 2005 and 2006. They have the same functions as a MDT6.0 exept some
> fancy interfaces.
> Unfortunately Autodesk ignored parametric surface module in next generation.
> So I'll stick to MDT6.0 for a while
> If you give me a few screen shots I'll appreciate, since I can not open your
> MDT 2006 or 2007.
> Regards
> Al
> "Bob Wiley" wrote in message
> news:5271708@discussion.autodesk.com...
>
> Alex and Jason,
>
> Take a look at this drawing it has the BOM functions I regularly use in
> addition to some that will do what Alex is
> looking for.
>
> Open this file and take a look at the BOM (AMBOM). Go all the way over to
> the right most 3 columns and you will see how
> I would format the size to drop the leading zero. The first of the three
> columns has the source size (1.476). The second
> has the unformatted calculated size in feet (ES) using the formula you
> provided. The third has
> the calculated size with
> the leading zero dropped. If you look at the formula in the third column,
> you will see that the unformatted size (ES) is
> referenced 3 times. If I had not placed the unformatted size in its own
> column then the formula in the third column
> would have been VERY long and hard to read.
>
> Now take a look at the column labeled "Size". It is fairly lengthy but is
> takes the X, Y, and Z dimensions for a
> rectangular part, sorts them, and puts them in my BOM. For this
> to work, My base extrusion must be a rectangle with
> constraints d0 and d1 as the length and width. When I extrude the rectangle,
> d2 is the draft angle which I ignore in the
> BOM. d3 is the extrusion distance. So it is d0, d1 and d3 that I sort and
> use. This works for most all of my parts.
> Anything that is not a rectangle to begin with requires me to manually type
> in the cut size on the BOM. The formula in
> this column is not locked so all I have to do is just type over the calcu
> lated cut size if needed.
>
> Look at the columns labeled "First space location" (SP), "PARSE" and
> "Description length" (US). These formulas set up to
> parse out the part number and description from the part name (File name). We
> add an "_S" on the end of all our 3D solid
> MDT files to distinquish them from regular Autocad 2D files. This "_S" is
> trimmed from the file name for the
> description. The formulas in columns labeled "Dwg/Part No." and
> "Description" use the formulas SP, PARSE
> and US to
> actually parse the part number and description. Normally I would have the
> SP, PARSE and US columns hidden but they are
> visible in this case just for discussions sake.
>
> The attached file is "SM-102002 CRANK GUARD COVER_S.dwg" The part number
> would be all the characters to the left of the
> first space. The description would be all of the remainder with the _S
> stripped away. I can't remember the last time I
> actually typed in a part number and description for a part. This
> works well!
>
> To make all these formulas easy to use requires they be inserted
> automatically. You don't want to have to type these in
> manually every time you need to use them. For some reason custom BOM
> standards cannot be put in your template file. What
> I have done instead is place them in a seperate file that can be inserted as
> a block into the current drawing. My BOM
> standard is in a file called SMNA_std_rev_B.dwg. I then have a toolbar
> button that fires the macro:
>
> ^C^C-i
> nsert "S:/TWOLF/DRAWINGS/LIBRARY/SMNA/TITLE/SMNA_std_rev_B" r 0 s 1
> 0,0,0;_amsymstd
>
> This inserts the drawing containing the BOM standard and runs AMSYMSTD so I
> can pick a specific BOM standard with it's
> associated formulas. I have three standards I use. One for parts, one for
> assemblies and one for purchased parts. These
> BOM standards also set up which columns show up on the parts list that is
> placed on the drawing.
>
> I have been using these BOM standards and formulas for probably
> 8 years now Obviously I did not do all this overnight
> and it has required some tweaking. The result has been untold hours saved
> and errors prevented.
>


--
Bob Wiley
Mechanical Designer

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 14 of 19
Anonymous
in reply to: Anonymous

Thanks Bob.
Al
"Bob Wiley" wrote in message
news:5308162@discussion.autodesk.com...
Alex,

I understand completely about using MDT6. It has not been that long since I
was forced to updrade here at work. I still
use MDT6 at home because like you, I find it more stable.

I hope the attached screen shots and spreadsheet will give you what you
need.

Bob


Alex wrote:

> I am still at MDT6.0 which I like better than next generations.
> I've been using a lot of lisp and some 3 party apps which not working with
> next MDT's
> but make my life a lot eazier.
> MDT6.0
is pretty much debugged and does pretty good job.
> I tried 2005 and 2006. They have the same functions as a MDT6.0 exept some
> fancy interfaces.
> Unfortunately Autodesk ignored parametric surface module in next
generation.
> So I'll stick to MDT6.0 for a while
> If you give me a few screen shots I'll appreciate, since I can not open
your
> MDT 2006 or 2007.
> Regards
> Al
> "Bob Wiley" wrote in message
> news:5271708@discussion.autodesk.com...
>

> Alex and Jason,
>
> Take a look at this drawing it has the BOM functions I regularly use in
> addition to some that will do what Alex is
> looking for.
>
> Open this file and take a look at the BOM (AMBOM). Go all the way over to
> the right most 3 columns and you will see how
> I would format the size to drop the leading zero. The first of the three
> columns has the source size (1.476). The second
> has the unformatted calculated size in feet (ES) using the formula you
> provided. Th
e third has
> the calculated size with
> the leading zero dropped. If you look at the formula in the third column,
> you will see that the unformatted size (ES) is
> referenced 3 times. If I had not placed the unformatted size in its own
> column then the formula in the third column
> would have been VERY long and hard to read.
>
> Now take a look at the column labeled "Size". It is fairly lengthy but is

> takes the X, Y, and Z dimensions for a
> rectangular part, sorts them, and puts them in
my BOM. For this
> to work, My base extrusion must be a rectangle with
> constraints d0 and d1 as the length and width. When I extrude the
rectangle,
> d2 is the draft angle which I ignore in the
> BOM. d3 is the extrusion distance. So it is d0, d1 and d3 that I sort and
> use. This works for most all of my parts.
> Anything that is not a rectangle to begin with requires me to manually
type
> in the cut size on the BOM. The formula in
> this column is not locked so all I have to do is just
type over the calcu
> lated cut size if needed.
>
> Look at the columns labeled "First space location" (SP), "PARSE" and
> "Description length" (US). These formulas set up to
> parse out the part number and description from the part name (File name).
We
> add an "_S" on the end of all our 3D solid
> MDT files to distinquish them from regular Autocad 2D files. This "_S" is
> trimmed from the file name for the
> description. The formulas in columns labeled "Dwg/Part No." and
> "Description"
use the formulas SP, PARSE
> and US to
> actually parse the part number and description. Normally I would have the
> SP, PARSE and US columns hidden but they are
> visible in this case just for discussions sake.
>
> The attached file is "SM-102002 CRANK GUARD COVER_S.dwg" The part number
> would be all the characters to the left of the
> first space. The description would be all of the remainder with the _S
> stripped away. I can't remember the last time I
> actually typed in a part number
and description for a part. This
> works well!
>
> To make all these formulas easy to use requires they be inserted
> automatically. You don't want to have to type these in
> manually every time you need to use them. For some reason custom BOM
> standards cannot be put in your template file. What
> I have done instead is place them in a seperate file that can be inserted
as
> a block into the current drawing. My BOM
> standard is in a file called SMNA_std_rev_B.dwg. I then have a toolbar
>
button that fires the macro:
>
> ^C^C-i
> nsert "S:/TWOLF/DRAWINGS/LIBRARY/SMNA/TITLE/SMNA_std_rev_B" r 0 s 1
> 0,0,0;_amsymstd
>
> This inserts the drawing containing the BOM standard and runs AMSYMSTD so
I
> can pick a specific BOM standard with it's
> associated formulas. I have three standards I use. One for parts, one for
> assemblies and one for purchased parts. These
> BOM standards also set up which columns show up on the parts list that is
> placed on the drawing.
>
> I
have been using these BOM standards and formulas for probably
> 8 years now Obviously I did not do all this overnight
> and it has required some tweaking. The result has been untold hours saved
> and errors prevented.
>


--
Bob Wiley
Mechanical Designer

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 15 of 19
.Peter
in reply to: Anonymous

Bob,

"Bob Wiley" wrote

>Anything that is not a rectangle to begin with requires me to manually type in the cut size on the BOM..

i have made a formula that works similar to yours, instead of using d0, d1, d3, i use AMVARS like PL, PW, PH, PD. With PD recognized in a part the Size will show the diameter.
i.e. =IF(LTE((TD),""),part:PL " x "part:PW " x " part:PH,"Ø " TD " x " TL)
results in Ø 10 x 10 if PD is detected, if not, L x W x H


>For some reason custom BOM standards cannot be put in your template file..

you can run AMSYMSTD in your Template file, right click your Standard and copy it with i.e. Part or assemblies or purchased parts name extension.
Then run amoptions standard tab, choose the copied standard and dblclick the node partlist. Edit the partlist to show the coloums to fit your need.
When using this template you can switch the Partlists with AMSYMSTD.


The MATERIAL i use from AMMASSPROP (mcad.mat) and submitted from VAL-table coloumn.
The WEIGHT i use a formula that uses PART:MASS (calculated from AMMASSPROP) which detects missing density
=IF(LTE((density),1),"nil",text(qty*PART:MASS,"0.00") & " kg")
To avoid weight display errors in BOM i have a Buttonmakro that update the ammassprop-calculation. Works fine for me.

I have a question at this point,
To avoid density errors and double work for Standarparts from amstdplib i´d like to assume the density from their VAL table.
Do you or anybody else know how to write the density from VAL table (G_RHO) to the density Attibute (amassign) of the part, as the Material-Value does?
The material is linked from Val-table to Bom-Value "Material1" and somehow to MDT-Part Attribute.
The density is sent by default from Val-table to amvars (G_RHO) and custumizeable linkable to the Standard BOM-Values, density is not an Optional Coloumn in Val-Editor.
Is there any way to write the G-RHO density from amvars or from Standard BOM-Value (i.E. User1-8) to MDT-Part Density?

Regards
Peter
Message 16 of 19
Anonymous
in reply to: Anonymous

Peter,


.Peter wrote:

> i have made a formula that works similar to yours, instead of using d0, d1, d3, i use AMVARS like PL, PW, PH, PD. With PD recognized in a part the Size will show the diameter.
> i.e. =IF(LTE((TD),""),part:PL " x "part:PW " x " part:PH,"Ø " TD " x " TL)
> results in Ø 10 x 10 if PD is detected, if not, L x W x H
This looks like would work very well. Plus you don't need to sort them like I do. I thought about using AMVARS similar
to that but 98% of my parts start out as an extruded rectangle so I never persued it.
>

>
>>For some reason custom BOM standards cannot be put in your template file..
>
> you can run AMSYMSTD in your Template file, right click your Standard and copy it with i.e. Part or assemblies or purchased parts name extension.
> Then run amoptions standard tab, choose the copied standard and dblclick the node partlist. Edit the partlist to show the coloums to fit your need.
> When using this template you can switch the Partlists with AMSYMSTD.
>
Yes I was incorrect in my reasoning for putting my standards in a seperate file as opposed to the template file. The
real reason I did this is it makes it easy to create a new standard and save it in a new "template" file with a new name
ie: ...REV_C. I can then insert this new template file as a block and have access to the new standard. What I really
should have said is you can't insert a standard as just a standard. It must be inserted using a drawing file as a
container. This is a requirement when using old files or library parts that may have none of my current BOM standards.
The only way to get the standards into these files is either to manually type it all in or insert them as part of a block.

>
> The MATERIAL i use from AMMASSPROP (mcad.mat) and submitted from VAL-table coloumn.
> The WEIGHT i use a formula that uses PART:MASS (calculated from AMMASSPROP) which detects missing density
> =IF(LTE((density),1),"nil",text(qty*PART:MASS,"0.00") & " kg")
> To avoid weight display errors in BOM i have a Buttonmakro that update the ammassprop-calculation. Works fine for me.
>
> I have a question at this point,
> To avoid density errors and double work for Standarparts from amstdplib i´d like to assume the density from their VAL table.
> Do you or anybody else know how to write the density from VAL table (G_RHO) to the density Attibute (amassign) of the part, as the Material-Value does?
> The material is linked from Val-table to Bom-Value "Material1" and somehow to MDT-Part Attribute.
> The density is sent by default from Val-table to amvars (G_RHO) and custumizeable linkable to the Standard BOM-Values, density is not an Optional Coloumn in Val-Editor.
> Is there any way to write the G-RHO density from amvars or from Standard BOM-Value (i.E. User1-8) to MDT-Part Density?
>

Now you lost me here. I am unfamiliar with what you refer to as the VAL-table column. Reason is I never use the standard
parts. They are usually just dumb solids and I spend way too much time getting the BOM information configured for each
part. Over the years I have created my own libraries of parts with real world BOM and mass property data. With very few
exceptions these days, when I insert a part out of my library it is 100% ready to go with BOM and mass property
information ready to go.

Fill me in a little on the VAL-table column.

--
Bob Wiley
Mechanical Designer

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 17 of 19
.Peter
in reply to: Anonymous

Hello Bob,


Bob wrote:

>> i have made a formula that works similar to yours, instead of using d0, d1, d3, i use AMVARS like PL, PW, PH, PD. With PD recognized in a part the Size will show the diameter.
>> i.e. =IF(LTE((TD),""),part:PL " x "part:PW " x " part:PH,"Ø " TD " x " TL)
>> results in Ø 10 x 10 if PD is detected, if not, L x W x H

>This looks like would work very well. Plus you don't need to sort them like I do. I thought about using AMVARS similar to that but 98% of my parts start out as an extruded rectangle so I never persued it.
>
Your solution with automatic variables save the work to use AMVARS, thanks for that input. I have setup the amvars in my template and in the AMOPTIONS,

Preferences Tab, Preset Values to have easier access to them. However, you could just use one amvar for the diameter to display round parts.
>>
>>>For some reason custom BOM standards cannot be put in your template file..
>>
>> you can run AMSYMSTD in your Template file, right click your Standard and copy it with i.e. Part or assemblies or purchased parts name extension.
>> Then run amoptions standard tab, choose the copied standard and dblclick the node partlist. Edit the partlist to show the coloums to fit your need.
>> When using this template you can switch the Partlists with AMSYMSTD.
>>
>Yes I was incorrect in my reasoning for putting my standards in a seperate file as opposed to the template file. The
>real reason I did this is it makes it easy to create a new standard and save it in a new "template" file with a new name
>ie: ...REV_C. I can then insert this new template file as a block and have access to the new standard. What I really
>should have said is you can't insert a standard as just a standard. It must be inserted using a drawing file as a
>container. This is a requirement when using old files or library parts that may have none of my current BOM standards.
>The only way to get the standards into these files is either to manually type it all in or insert them as part of a block.

I use AMSETUPDWG for such cases and choose the template with the standard.

>>
>> The MATERIAL i use from AMMASSPROP (mcad.mat) and submitted from VAL-table coloumn.
>> The WEIGHT i use a formula that uses PART:MASS (calculated from AMMASSPROP) which detects missing density
>> =IF(LTE((density),1),"nil",text(qty*PART:MASS,"0.00") & " kg")
>> To avoid weight display errors in BOM i have a Buttonmakro that update the ammassprop-calculation. Works fine for me.
>>
>> I have a question at this point,
>> To avoid density errors and double work for Standarparts from amstdplib i´d like to assume the density from their VAL table.
>> Do you or anybody else know how to write the density from VAL table (G_RHO) to the density Attibute (amassign) of the part, as the Material-Value does?
>> The material is linked from Val-table to Bom-Value "Material1" and somehow to MDT-Part Attribute.
>> The density is sent by default from Val-table to amvars (G_RHO) and custumizeable linkable to the Standard BOM-Values, density is not an Optional Coloumn in Val-Editor.
>> Is there any way to write the G-RHO density from amvars or from Standard BOM-Value (i.E. User1-8) to MDT-Part Density?
>>

>Now you lost me here. I am unfamiliar with what you refer to as the VAL-table column. Reason is I never use the standard
>parts. They are usually just dumb solids and I spend way too much time getting the BOM information configured for each
>part. Over the years I have created my own libraries of parts with real world BOM and mass property data. With very few
>exceptions these days, when I insert a part out of my library it is 100% ready to go with BOM and mass property
>information ready to go.

The BOM-information for the standard Parts is just one advantage for me of using standard parts. Even some of them are baseparts you can ampoweredit (or dblclick) them to choose another size from VAL-Table-Row. BOM-Info changes parametric. You can also work on the part with parametric features or even edit the basepart with a special BASE-Part-editing Toolbar.


>Fill me in a little on the VAL-table column.

If unknown, this (Optimizing Standard Parts) should fill you in a little.
http://usa.autodesk.com/adsk/servlet/link?siteID=123112&id=5357858&linkID=4183230
to see to which column of your BOM you can link a VAL column check Page 13 #7.
Check the dropdownfield marked with the blue arrow .
This example is for a new Column, existing VAL columns you can link to your BOM by activate the column and hit Strg+T
--

Best Regards
Peter
Message 18 of 19
Anonymous
in reply to: Anonymous

Thanks Peter,

.Peter wrote:

> If unknown, this (Optimizing Standard Parts) should fill you in a little.
> http://usa.autodesk.com/adsk/servlet/link?siteID=123112&id=5357858&linkID=4183230
> to see to which column of your BOM you can link a VAL column check Page 13 #7.
> Check the dropdownfield marked with the blue arrow .
> This example is for a new Column, existing VAL columns you can link to your BOM by activate the column and hit Strg+T
GREAT GOOGLY WOOGLY... How in the world after all these years of using ACAD and MDT did I miss all of that! This opens
up a lot of new opertunities. For the moment I can't answer your question but you can bet I'll be customizing the
standard parts and using them in the future.

Bob

--
Bob Wiley
Mechanical Designer

IV 10 SP3a
MDT2006 SP2
Vault 5
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, driver version 81.72
Message 19 of 19
TroyNageotte
in reply to: Anonymous

Bob & Jason,

Thanks so much for taking the time to post this string. It is very helpful and explains things that I have struggled with for years. I find it strange the command "amsymstd" is not even listed in the command references for MDT. I have been maintaining multiple templates to create different style of parts list. I also really appreciate the formulas for a cutting list.

Troy Nageotte
Inventor Professional 11 SP3
MDT 2007 SP2
CAD Manager
Watchtower
Troy Nageotte
Inv Pro 2011
MDT 2009 SP3
Mechanical 2011
Design Review 2011
Microsoft Forefront 1.61 (antivirus scan)
Windows 7 x64
Intel Core 2 Duo 3.00Gzh 8.0 GB RAM
nVidia Geforce GT 430 1 GB

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