volume note on a drawing

[JMSCRA]

OK I give up! ;^(

I am trying to create a note on a drawing that displays the volume of the part that drives the drawing.
I have tried a number of things with no luck.
Please help.

WF5.0 & PDMLink 9.1

John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CCB5A6.989C9920]
________________________________

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[TedOtto]

I use:
&PRO_MP_VOLUME
&PRO_MP_MASS


Ted

[DonSenchuk]

Without more details on what you've tried already...

Insert this into your note: &pro_mp_volume

In Reply to John Scranton:

OK I give up! ;^(

I am trying to create a note on a drawing that displays the volume of the part that drives the drawing.
I have tried a number of things with no luck.
Please help.

WF5.0 & PDMLink 9.1

John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CCB5A6.989C9920]
________________________________

[BenLoosli]

They must be in a table to update.

Thank you,

Ben H. Loosli
USEC, INC.

[dgschaefer]

Not true, they only need to be in a table if they are placed in a
format. Parameters in standard drawing notes should update.



If that's not working, check that a mass props analysis has been run and
perhaps set 'mass_property_calculate' to 'automatic' to insure that it's
always up to date. Also, you may have troubles if your drawing has
multiple models. Make sure your main model is active before creating
the note.



Doug Schaefer

[davehaigh]

If you download my talk ProE Admin 101 there is a movie file in there that goes over how to show the mass of a part in a note on the drawing. You would use the same method to do the volume. If it's something you do a lot, you can add it to your start part.


ProE Admin 101

[ptc-2860737]

Yes, you need to be careful when using mass_property_calculate because if
it's not set to automatic then the mass properties (&pro_mp_volume, etc.)
are stale. And you may find that you don't want mass_property_calculate
set to automatic (as in our case, but I won't get into that).

What we do is create a mass properties feature in the model, place it in
the footer so that it's always current, and then you can use the
parameters out of the analysis feature (such as volume) in a drawing note
using the format &volume:fid_<place the=" name=" of=" the=" feature=" here=">.


Doug Barton
Senior Mechanical Designer
Parker Hannifin Canada
Electronic Controls Division
1305 Clarence Avenue
Winnipeg, MB R3T 1T4 Canada
direct 204 453 3339 x309
fax 204 452 7156
-
www.parker.com/ecd

[JMSCRA]

I have tested them in and out of a table and neither of those will update when the part changes.
I have updated the table and sheets in the drawing after a model change with no affect. I have regenerated the model form the drawing. Again no update to the note.


John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CCB5B9.B73D5910]

[JMSCRA]

Setting the option 'mass_property_calculate' to 'automatic' does work but then we will be calculating mass properties every time a change is made on every part. That does not sound like that is making good use of resources. In fact if my memory serves me correctly I had the option set that way some time ago and changed it because of the problems that caused.

The issue here is that with the option set to "by request" it does not update the note or table no matter how many times things are updated or regenerated or the mass properties are calculated. Do we have a bug in WF5.0?

John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CCB5BA.D706BFB0]

[ptc-2860737]

It's not a bug, it's just another quirky bit of Pro/E behavior, and it is
documented in the help files.

Running Analysis > Model > Mass Properties does not update &pro_mp_volume
(mass, etc.). And is temporary data unless you create an analysis
feature.

To update &pro_mp_volume (mass, etc.) you need to either have config
option mass_property_calculate set to automatic (which as John suggests
and we discovered is not always desirable) or generate a mass properties
report using Edit > Setup > Mass Props > Generate Report (which is a one
shot deal so &pro_mp_volume quickly becomes stale).

To get around using &pro_mp_volume and have current mass properties data
you can create an analysis feature and place it in the footer of the model
tree so it is calculated after part regeneration. Then you can use the
parameters create by the analysis feature (such as &volume:fid_<place the=" <br="/>name (or feature ID) of the feature here>).


Doug Barton
Senior Mechanical Designer
Parker Hannifin Canada
Electronic Controls Division
1305 Clarence Avenue
Winnipeg, MB R3T 1T4 Canada
direct 204 453 3339 x309
fax 204 452 7156
-
www.parker.com/ecd

[DonSenchuk]

Ever see a post where someone mentions a feature not working as expected then wonder how many people scramble to test it out themselves?

Anyway, a couple of quick tests leads to the following...

Adding to what Doug mentions in his post, leaving 'mass_property_calculate' set to 'by_request' leaves only one way to get the note to update (that I found in a quick test). After the model changes and has been regenerated, you have to go to Edit > Setup > Mass Props and pick Generate Report. Doing so forces a note using &pro_mp_volume to adopt the new value.

The best option is to use the analysis feature Doug outlined.

In Reply to John Scranton:

Setting the option 'mass_property_calculate' to 'automatic' does work but then we will be calculating mass properties every time a change is made on every part. That does not sound like that is making good use of resources. In fact if my memory serves me correctly I had the option set that way some time ago and changed it because of the problems that caused.

The issue here is that with the option set to "by request" it does not update the note or table no matter how many times things are updated or regenerated or the mass properties are calculated. Do we have a bug in WF5.0?

John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CCB5BA.D706BFB0]

[ptc-141274]

I should have mentioned that I was on WF4, but it seems that it might not have mattered.

At this point there is not an elegant solution, but an acceptable workaround.

A couple people suggested to click the ALL SHEETS IN PAPER SPACE button, on the SHEETS tab in the DXF export dialog box. This gives me one file with the sheets on different tabs. I tried to open it up in Autocad but for some reason I could only see one sheet.

I have another department trying out the file as well, but my suspicions are that all our downstream applications will not like this file. We have been using one separate DXF file for each sheet for ever.

Thanks to Jim for the work around!

The mapkey does change sheets for you. The non elegant part is that it goes thru a non-intelligent loop until it comes around to the first sheet, and then you manually have to cancel it. I can live with that though.

I think to get to a more elegant solution, would take some of the higher level coding in Pro-E.

Doug

[davehaigh]

First you need to create the mass prop feature correctly

1. the proper way to create a mass property feature is create it and then put it in the footer of the part or assembly. That way it's always the last feature in the part.

2. You need these two config options

a. Mass_property_calculate automatic

b. Relations_unit_sensitive yes

3. When you create the mass prop feature you need to make sure that you set regenerate to "Always"

4. Create feature relations & parameters to report the mass props in the units you want. (See the video in ProE Admin 101)

5. Show it in a note on the drawing or in the model like this xx. Estimated weight is &<feature parameter=" name=">:FID_<mass prop=" feature=" name=">[.2]

a. If you use the mass prop feature name ProE will populate it with the correct feature ID.

Most of the issues people complain about when using mass_property_calculate automatic have to do with family tables and have been resolved in later revs or ProE.

Family Tables issues can be resolved by setting these options.

1. The family table has to be verified when the option mass_property_caluclate is set to automatic

2. If you're on wf3 there is a hidden option mark_insts_modified_by_mp_calc set it to changed.

3. Set verify_on_save_by_default to yes

4. Set relat_marks_obj_modified to no

5. Set bump_revnum_on_retr_regen to no

6. Set regen_read_only_insts to no

7. Set regenerate_read_only_objects to NO

8. Set save_objects to CHANGED

David Haigh

[FredericVannest]

An extra question regarding this one...
Anyone find a good way to add the unit of these parameters
parametrically to the note???
The unit is there in the parameter but we are looking for a way to
access it so we can add it to the note.

Kind regards,

Frederic

[davehaigh]

Perhaps the description field can be accessed. Not sure how to do that.

[cid:image001.png@01CCB649.400E7960]

David Haigh

[MikeBrattoli]

You can populate the units for a parameter defined in a material file into a repeat region. It won't say "pounds" but it will show the units currently set for the model "lbm", "kg", etc...

Go to your material library and add a user defined parameter to a material (I just created one called WEIGHT_UNIT), gave it a Description of Pounds, and set the Unit to lbm

[cid:image001.jpg@01CCB67C.75B751D0]

Create a repeat region in your drawing format and select "mdl.param.unit" in the cell. When you change the units in your model the repeat region value will automatically update the next time the drawing is opened/updated

[cid:image002.jpg@01CCB67C.75B751D0][cid:image007.jpg@01CCB67C.75B751D0][cid:image014.jpg@01CCB67C.75B751D0]

Might be a way to capture that in a drawing note (haven't figured that one out yet) but at least you could capture the mass units of your part in our drawing format

My 2 cents 🙂

Mike Brattoli
Moen Incorporated
Global Strategic Development
Engineering Systems Administrator
E

[MikeBrattoli]

I misspoke on one thing - create a string parameter in the material with the word "pounds" or "kilograms", etc.... then put "material.param.mass_unit" with a string value of "Pounds (lbs)" - (mass_unit is the user defined parameter in the material file) into the repeat region - you get this

[cid:image001.jpg@01CCB67E.12FAC2A0][cid:image002.jpg@01CCB67E.12FAC2A0]

Mike Brattoli
Moen Incorporated
Global Strategic Development
Engineering Systems Administrator

[DonSenchuk]

Mike mentions (in the quoted reply) there might be a way to get that into a drawing note.

There is a way to get material parameters into a normal note. (Note these instructions are for WF4.0)

These take place after creating a parameter in the material as per Mike's instructions.

1. PickTools > Relations.

2.Pick the 'Insert Parameter Name from List' icon. (It looks like a pair of parentheses.)

3. Change the 'Look In' pull down menu from Part to Material.

4. Select the material and pick the OK button.

5. You can now see the parameter you added to the material per MIke's instructions. Select it and pick the Insert Selected button.

Your relations will display the string necessary to enter the value into a note. Something similar to

Go to your material library and add a user defined parameter to a material (I just created one called WEIGHT_UNIT), gave it a Description of Pounds, and set the Unit to lbm

[cid:image001.jpg@01CCB67C.75B751D0]

Create a repeat region in your drawing format and select "mdl.param.unit" in the cell. When you change the units in your model the repeat region value will automatically update the next time the drawing is opened/updated

[cid:image002.jpg@01CCB67C.75B751D0][cid:image007.jpg@01CCB67C.75B751D0][cid:image014.jpg@01CCB67C.75B751D0]

Might be a way to capture that in a drawing note (haven't figured that one out yet) but at least you could capture the mass units of your part in our drawing format

My 2 cents 🙂

Mike Brattoli
Moen Incorporated
Global Strategic Development
Engineering Systems Administrator

________________________________________________________________

[davehaigh]

The original question was how to get the units in the mass prop feature parameters into a note. That's fundamentally different than displaying the material user defined parameters in a note.

Your material may be defined in g/cc, but if you apply that material to a part that is inchs, ProE will automatically convert the values, but I doubt it's going to know how to convert the user defined parameter. So you would have a problem in that case.

The mass prop feature parameters can have a unit assigned to them so regardless of the units of your model you can put a not on the drawing that shows both English and metric values. The question was can you grab the value assigned to that feature parameter and display that automatically rather than just dumb text in the note.

In this screen shot the part is in English units, but I've defined both kg and grams as the units for two of the feature parameters. I've also added information in the description field. The question is how do you access the information in that description field.
[cid:image001.png@01CCB66A.C482D940]

David Haigh

[MikeBrattoli]

Don, I totally agree about entering the text manually. I would avoid the repeat region, etc... and put it into the note as you listed

I'm using WF 5.0 and the info shown below worked fine - nice. Here's what it told me for the material parameter MASS_UNIT:MTRL_242 and the drawing note I typed in was "UNITS OF WEIGHT: &MASS_UNIT:MTRL_242". It displayed on my drawing as "UNITS OF WEIGHT: POUNDS".

I'm of the opinion that capturing the "value" (POUNDS, KILOGRAMS, etc...) in the material file not only encourages the designer/engineer to assign a material to a file (instead of just enter text or a density value) and ensures consistency.

Since it would also work in a repeat region as I described that would be a way to capture that for say an assembly with mixed units.

A successful Friday afternoon - I can go home now 🙂

Thanks Don!

Mike Brattoli
Moen Incorporated
Global Strategic Development
Engineering Systems Administrator