Summation of weight parameter in repeat region not taking into account qty of bom item

[KDobie13]

I am using Creo Parametric Release 8.0 and Datecode8.0.11.0

I am trying to add a weight per piece column into our bill of material in the repeat region on our drawing format. I successfully added a column that pulls from our weight parameter in the part but when I add the summation to the repeat region for total weight it only adds the weight per piece once and is not taking into account the quantity of the part.

I also would like to know if it is possible to put this summation into a different table in the drawing that is not part of the repeat region. I tried adding the summation string to another table in the drawing but it does not work like intended. I can type the parameter into the drawing manually and it adds it but not permanently in the format.

Lastly would like to make it so that the balloons are always set to "QTY SPLIT" when making a new drawing instead of having to change it.

[MartinHanak · Accepted solution]

Hi,

answer to Q1:

1.] add relation into repeat region ... full_weight = rpt_qty * asm_mbr_weight

2.] add new column into repeat region ... &rpt.rel.full_weight

3.] add summation to above mentioned column

answer to Q2:

AFAIK summation formula belongs to specific repeat region. You cannot place it into separate table.

answer to Q3:

https://www.creosite.com/cgi-bin/find_option.cgi?srch=default_bom_balloon_type&ver=creo1&mode=drwsetup

[KDobie13]

Thank you Martin. If I want to keep the column in the repeat region as weight per piece is it still possible to add this relation and do a summation in another way? The company that owns ours does this and I can't seem to figure out how they do it. Unfortunately, the person I used to ask for these things is no longer with the company.

In regards to Q3 this is a config change then and not a drawing template change?

[Mahesh_Sharma]

Hi @KD_12152530 

Will it be possible for you to share a sample data to check how was it done?

For summation of weight of all instances, a column is required which can further be used to calculate total weigh.

Thanks.  

[StephenW]

If you attached a picture of what you wanted (or what your company already has) and a the use switch symbols in the table and add another picture (you may have to widen the columns to make it readable) and then a picture of repeat region relations.

For example (my example doesn't have relations/parameters):

[KDobie13]

Stephen,

When I switch symbols all it says is "&TOTAL_WEIGHT:D[.1]"

This parameter is only in the drawing parameters and not the part parameters.

Is there a way to see the way this summation was created? I put my test assembly on both drawing templates and the BOM operates correctly and shows the weight/piece which is derived from our part parameter "WEIGHT_KG" but my summation does not take into account quantity.

This is the only table on the format I blanked some thing because I am not sure what I am allowed to share.

[StephenW]

Ok, There are several things happening here, lets work thru understanding them separately.

The repeat region is the area that has the magenta box outline and is NOT related to the other portions of your title block, such as the total weight field.

Your total weight field is interesting. The : D(colon D) at the end of the parameter name means it comes from the drawing (not the model as I would have guessed). So, within the drawing, there is something going on that takes the model weight and converts it to drawing parameter. I am guessing, since its not something I have done, that your company uses a Drawing Program to do this. You can view the drawing programs, in the drawing, under Tools, Drawing Program, Edit Program. This is really a guess, but that looks like the next piece of information we need to figure out your title block.

What is your "end goal"? I re-read your initial post and I don't understand what and where you are really trying to do.

[KDobie13]

I checked and there are no drawing programs.

The total weight parameter is created in the repeat region menu using the summation option. This is what I understood at least. Once you pick something to be summed you need to name the parameter and then pick a cell for it to go into inside the same table that the repeat region is a part of.

The goal is to have the BOM column show weight/piece and then have a total weight that is shown in the title block like the picture above. The problem I am having is that when I create the summation it adds the weight/piece column but only in quanitity 1 and not how many are actually in the assembly. So it will add component one as 5 kg even if there are 5 pieces where it should say 25kg total.

[StephenW]

Hmmm, I didn't realize summation worked that way, that's a new one for me. To be honest, I haven't used summation in a long time. So I don't know the answer to your problem with summation.

So, my next question is why are your using summation at all instead of just using the mass from the assembly. Maybe I'm missing some other purpose?

We use &pro_mp_mass in the title block to get the mass from the model. This is a mass parameter from the model and has nothing to do with repeat regions.

Does that solve your problem?

To test, just make sure the active model is your assembly, then make a note in the drawing with &pro_mp_mass

[KDobie13]

Stephen,

I just figured it out. I found a relation in the repeat region menu.

Also as for not using the the assembly weight that is because a lot of our assemblies have what we call a "suppressed assembly" inside of them that we put objects into that we don't want to show in the BOM but we want to be able to see as a representation. Like a machine frame being used to show where covers get mounted to. We only want the covers in the BOM and the weight of the covers excluding the frame so this is why we want a summation of just the drawing weights.

As for why we use a "weight_kg" parameter I am not totally sure maybe to help with the described above task. I know this parameter is used directly to import the weight into our ERP system, It has been this way since I started here and unfortunately the gentlemen responsible for all this passed away so I do not have him to ask for help anymore.

The weight_kg is calculate with "WEIGHT_KG=ceil((1000*PRO_MP_MASS),1)" in our default part template.

edit. I also think this relation is what Martin the first responder suggested but I want to still keep the weight/piece in the column. I can recreate the relation and keep it in the background then do a summation of the parameter to get total weight in the title block.

[KDobie13]

Martin,

I can only get the Total_weight to sum properly if there is a column for the relation. Is there a way around this?

Thanks,

Kyle

[StephenW]

My hack work-around I've used in the past for something similar is to make the column really small width and make the text really small, so the column is there and is usable, but is pretty much invisible.

[KDobie13]

Hey Stephen,

This trick is what the other format I have been referencing does as well. Problem is the text is super small but still shows up as a dot on the pdf when generated. Oh well.

Sorry to piggyback off this post but I was successfully able to finish or D sized format. Problem is when I went to do our C I copied the tables over to the C from the D and now I am getting extra tables showing up. The blank format looks correct but it seems when I go to use the format older tables are getting pulled from. I tested this by wiping the complete format except for the border and when I add an assembly to it tables are appearing from somewhere. Any idea what could be happening here?

Thanks

[StephenW]

You'll likely get better answers if you make a new post. It's a different topic and will likely get you confusing answers.

I don't have a clue what is happening with your format, to be honest!

[MartinHanak]

---

@KDobie13 wrote:

Hey Stephen,

This trick is what the other format I have been referencing does as well. Problem is the text is super small but still shows up as a dot on the pdf when generated. Oh well.

Sorry to piggyback off this post but I was successfully able to finish or D sized format. Problem is when I went to do our C I copied the tables over to the C from the D and now I am getting extra tables showing up. The blank format looks correct but it seems when I go to use the format older tables are getting pulled from. I tested this by wiping the complete format except for the border and when I add an assembly to it tables are appearing from somewhere. Any idea what could be happening here?

Thanks

---

Hi,

if the (.frm) format contains a table and the user creates a new drawing using this format then Creo copies the tables from the format to the drawing. These copied tables are independent of the tables in the format. If you later change the tables in the format, then this change will not be reflected in the existing drawings.

I recommend that you follow the following rules.

1.]

If a change needs to be made to the format, then make a new version of the format and give it a different name.

Eg. myformat_v1.frm, myformat_v2.frm and so on.

2.]

If it is necessary to change the format in an existing drawing, then do not forget to delete all tables belonging to the previous version of the format.

[KDobie13]

Martin,

I understand what you mean that existing drawings will not get new changes to the format unless you manually updated the old drawings with the new format.

The problem that I currently have is this. I view the format and this is what I see. Blank with no tables

When I go to use this format it is pulling old incomplete tables and sketched entities from somewhere else.

This is very odd. I can start a new thread if you like.

Thanks,
Kyle Dobie

[MartinHanak]

---

@KDobie13 wrote:

Martin,

I understand what you mean that existing drawings will not get new changes to the format unless you manually updated the old drawings with the new format.

The problem that I currently have is this. I view the format and this is what I see. Blank with no tables

When I go to use this format it is pulling old incomplete tables and sketched entities from somewhere else.

This is very odd. I can start a new thread if you like.

Thanks,
Kyle Dobie

---

Hi,

please provide detailed description how do you create new drawing. Publish a picture for every single step.

Also:

1.]

Please find config.pro option pro_format_dir and publish its settings.

2.]

Execute following test:

• start Creo
• open empty format shown in the first picture
• create new drawing ... I expect Creo will use format opened in previous step

[KDobie13]

Unfortunately I have checked in the changes to this template so if I need to go backwards I may need to start over or create a copy of a previous version that was known working. I also tested this on a coworkers computer and the issue persists when they try and use this template.

I created a new workspace to go through the next steps. Just blanking company name because I am not sure how much I am allowed to share.

File New/Drawing/Use default template/ok

Empty with format/browse/type in the format name/ok (usually it would be shown in this folder but they were moved for permission reasons to edit. the ones shown are bad copies with underscores in name)

Drawing shows up and has a bunch of extra tables in it. Double repeat region and title block etc

1)  Our templates are pulling from a directory in Windchill.

2) I did try this and had the same results.

[MartinHanak]

---

@KDobie13 wrote:

Unfortunately I have checked in the changes to this template so if I need to go backwards I may need to start over or create a copy of a previous version that was known working. I also tested this on a coworkers computer and the issue persists when they try and use this template.

I created a new workspace to go through the next steps. Just blanking company name because I am not sure how much I am allowed to share.

File New/Drawing/Use default template/ok

Empty with format/browse/type in the format name/ok (usually it would be shown in this folder but they were moved for permission reasons to edit. the ones shown are bad copies with underscores in name)

Drawing shows up and has a bunch of extra tables in it. Double repeat region and title block etc

1)  Our templates are pulling from a directory in Windchill.

2) I did try this and had the same results.

---

Hi,

it seems to me that you are somewhat confused and do not understand my instructions.

1.]

Do not use the term template.

In Creo terminology template and format are different objects!

2.]

Try again my test:

• start Creo
• open empty format shown in the first picture
• create new drawing ... I expect Creo will use format opened in previous step
  • when selecting the format, switch Open  window from  User format  to In session (see following picture)

[KDobie13]

Hello Martin,

I apologize for the confusion in my terminology. Unfortunately this still did not work. I am concerned there is a location somewhere on our network that there is information being pulled from unintentionally. I will have to continue doing some testing.

I did notice now though that the changes I made to the D size are affecting existing drawings. I should have created a V2 template as you suggested but I had already checked in my work.  I think the best is to revert to the last working format of each size and make new copies and focus on making these correct without messing up the existing format.

Is there a good way to revert to an old iteration in windchill?

Regards,

Kyle

[StephenW]

@KDobie13 

You may have rights to delete versions of files in the commonspace

-or-

I would suggest:

Make an empty workspace

search the commonspace for the format(s).

open the information on the format

select the "i" on the format  version that you want

Go to action - add to workspace

make sure it says "as stored", if not, set it to as stored.

then okay to add the old format to the workspace (should show as out of date once added)

unlock in your workspace if you use an auto lock on add function

open the format in creo (should show as old format)

then, go back to the workspace, update to format using the update - out of date versions command, BUT do not let it replace what is in memory with the latest version.

SAVE  the old version in creo (verify it saved, if necessary, make a minor edit to the format then save again)

check out the modified format in your workspace (don't overwrite your modification by allowing it to download the format again)

then check it in

[KDobie13]

Thank you Stephen this worked and seems to be back to the old working version of our C sized format. I never was able to figure out why I was getting these mysterious tables showing up in new drawings when the format was completely blank but I will have to do some playing around to see if I can figure it out. Going to save copies going forward to do testing.

[MartinHanak]

---

@KDobie13 wrote:

Martin,

I can only get the Total_weight to sum properly if there is a column for the relation. Is there a way around this?

Thanks,

Kyle

---

Hi,

I don't think it exists.

[KDobie13]

Hi Martin,

In regards to point 3 is this something that needs to be added to our default creo config file or is this something specific to each format?

Regards,

Kyle

[MartinHanak]

---

@KDobie13 wrote:

Hi Martin,

In regards to point 3 is this something that needs to be added to our default creo config file or is this something specific to each format?

Regards,

Kyle

---

Hi,

it is necessary that you always communicate exactly what you are asking.

I don't know what point 3 you are talking about.

[KDobie13]

I hit reply on your original comment so not sure how it was not visible. It's the point about changing default balloon display to quantity split circle. Do I need to update the .dtl file and then update that file on the drawing format?

[MartinHanak]

---

@KDobie13 wrote:

I hit reply on your original comment so not sure how it was not visible. It's the point about changing default balloon display to quantity split circle. Do I need to update the .dtl file and then update that file on the drawing format?

---

Hi,

BenLoosli already answered your question ... 2024-10-30 07:01 PM

[BenLoosli]

If you are referring to the split qty balloons, it is  .dtl setting (Drawing Setup) applied to your drawing templates.

[KDobie13]

Do I need to update the .dtl file and then update that file on the drawing format?

[BenLoosli]

Yes, edit the file and them load it into the drawing format and/or drawing template.