BOM Balloons for simplified reps!

[PrebenReventlow]

Hi

We have some fairly large assemblies which we want to show on a drawing.

The problem is that on sheet 1 we use a simplified rep called Default with a BOM and BOM Balloons.

On sheet 2 we have a simplified rep called Inspection_side with several components hided.

We want to use the numbers from the BOM on sheet 1 to show up on Balloons on sheet 2.

OTB it's not possible, but have any of you some good ideas??

[DomenicLaritz]

We often have the same problem - and also no useful solution!

Always doing double work on two repeat regions.

[PrebenReventlow · Accepted solution]

We dug a little deeper and found a solution.

Layout Tab > Format section > Component Display > Blank.

Not the most sophisticated solution, but it works well for us.

You can pick the model in the view or in the browser.

Now you can keep the same Simp Rep and just "adjust" it a little bit.

[DomenicLaritz]

The problem is, if somebody else has to make a modification on the drawing, he only on closer inspection recognizes, that components in a view have been blanked.

We're using WF4 - maybe in the drawing model tree (since WF5) this can be regognized better?!

One way or another, PTC please provide us a solution!

[dgrobe]

just to add to this.. in the component display box.. if you select all views.. the items you click.. will hide on all sheets, and views..  this could come in handy

[travisrd]

Thank you very much for that. 

I used this, in conjunction with another trick, to show varied positions on a mechanism with springs. 

The trick was to make a spring assembly, with more than one spring in it (uncompressed, compressed, somewhere mid-stroke), all mated to a common end face, and hide the one(s) that shouldn't be seen.  That spring assembly is used, with BOM parameters indicating its a spring component, not an assembly.  Mass props can be reduced by number of springs. 

What I didn't know how to do was to hide them.  Layout>Edit>Component Display>Blank was my missing piece. 

Again, thank you very much.

[AldoSouza]

Hi ,

In my opinion using index for balloons is not very reliable, even for one single table, if you have simp rep it will become worse.

My suggestion -

1- Create a string parameter you models . "pos" for example.

2- Instead of index column use "asm.mbr.pos" as parameter in the repeat region

3- Create a Custom Balloon symbol , or a copy from the existing one.

4- If copied, edit the copied symbol and replace where is "\index\" by "\asm.mbr.pos\".

5- Use that custom balloon symbol to show your balloons from repeat regions.....

That way you won't need to worry about fix/unfix. Each components will have its own position, no matter what simp. rep you are using.

Also you are able capture the value for that "pos" parameter from your file number if you want to.

Think about that.

Regards

[JavierGarcia]

I have used the technique you are talking about and it works but it has got some problems. For example, we use fasteners that don´t have any numbers, the file name can be: DIN912_M10x50. With these fasteners or other commercial items we don´t have any numbers to capture your "pos" from...

Regards

[ThibaultDubuis]

Hello,

I recently found a nice behavior of ProE regarding Pro/report and SimpRep that could solve your issue:

1) Create a "temp" simprep with all comps as MasterRep.

2) Create a "temp" drw with a view of the ASM + ReportTable (related to the "temp" SimpRep)

--> Fix all Indexes of the region

--> Create balloons for all

--> SAve your temp drawing

--> Erase the Temp Drawing from memory

3) Delete the "temp" SimpRep from your ASM

4) Create your Final Drawing

5) Import (merge) the temp DRW in your Final Drawing

The trick is here: As the "Temp" SimpRep does exists anymore, ProE asks to select another SimpRep to replace it !

--> You Merge the Temp drawing twice and your job is done !

Hope this helps.

Thibault

[Patriot_1776]

If you have a stand alone "repeat-region-type" BOM table, as I've made, the simplified rep that is active when you insert the table is the one that populates the table. You can then "fix index" to get all the parts to match the "master" BOM on sheet 1. Fixing indexes is easy and should always be done anyways because if you go changing the order of the parts in the model tree, it will affect the master BOM anyways, leading to issues with notes referencing certain item numbers. In my opinion, fixing indexes is mandatory, and would solve your problem as well. It's also extremely simple.

[Spencer_Brock]

Does fixing the index allow you to redistribute quantities between balloons from the different reps?

[wbottis]

it's extremely simple and therefore you don't want to explain how to do it?

[StephenW]

Fix index is under table - repeat region fix index. 

It's a manual process that is "easy" for a few items in a BOM but if you have 100's, you have to match them manually, its pretty tedious.

There used to be a work-around but the last time I tried it, I couldn't get it to work. You can try it https://community.ptc.com/t5/Creo-Parametric-Ideas/Allow-BOM-Ballons-from-Master-Rep-Repeat-Region-to-be-displayed/idc-p/466857/highlight/true#M5732 See Chris3 's post. It uses edit attachment-"same ref" option.

While you are in that post, vote for the product improvement idea. Not that it will get fixed but it's all we can do to try to get PTC's attention.

[wbottis]

I fixed a few indices, then changed the simplified rep of the table, and all the indices re-sorted anyway.  I have no sorting in the table assigned...wth

[StephenW]

I don't think I have ever change the rep on one after I set the rep. I usually make sure I have the rep set to the one I want and then use fix index.

[wbottis]

I might be missing the point here.  If I have a multi-sheet drawing where some views use the master rep, and others use simplified reps, my goal would be to maintain the order of the find numbers (i.e. "index numbers") and corresponding part numbers throughout the drawing regardless of the view, sheet, or number of items in the BOM table for that sheet.  That is the goal.  How do you accomplish this?

[StephenW]

PTC is missing the point. There is no reasonable way to do this. Using different simplified reps in a drawing doesn't let you move balloons from one view to a different one with a different rep. They don't make it easy at all to have matching balloons in multiple BOM tables. 

Your WORK-AROUND options are all poor:

1. you can try the edit attachment "bug" using the "same reference" option (that may or may not work anymore) this option would use one master BOM on the drawing, regardless of simplified rep, which in my opinon is the right way to do it

2. you can make a bom table for each sheet (each rep) and manually match the the bom index numbers for each item in the tables using the fix index command (apparently after setting the rep of the table based on your experience)

3. You can try using the component parameter option to use a manually set component parameter for each item in the assembly (instead of the automatic index number) and then make a custom bom balloon that finds the component parameter instead of the index number. There was a post that explained this process but I couldn't find it right off hand, it's a very specific parameter type that only exists in only in assemblies.

4. Completely manual balloons 

I wish I had a real, actually good solution for you.

[Chris3]

Steve has the right answer here. He has indicated the options, none of which are good. The "same reference" technique was "fixed" in Creo 4 (no longer possible).

[wbottis]

so, they "fixed" the best workaround by eliminating it?

[tnguyen-7]

I stuck with this problem for the whole day. This is what I done so far.

Repeat Region  - Model/Rep - (click on your region) then link to your Assembly file. On open rep windows choose you Rep that you want to show on that detail drawing.

Your table region is updated to your Rep and you can now create BOM balloon without effected your master assembly drawing.

[vcrawford]

I have figured out the same thing only recently. but have added a table on the sheet showing the simp rep, named that simp rep. and then hide the table. it is outside of the drawing frame. the other bonus to doing this is that your table only shows what is in the rep and its qty. so if you have 50 washers of on number the table and balloon only displays the qty in the rep. ie 12.

[AmiHalfon]

Thank, this is exactly what i done and it worked perfectly

[wbottis]

Yes, but the BOM table for the "simplified rep view" includes only those items reporting to the simp rep, so the Find Numbers are then hosed.  How is this beneficial?