1-Visitor

Question

Create a BOM index between Simplified reps

Forum|Forum|10 years ago
June 24, 2015
4 replies
20224 views

Hello,

My company is trying to create drawings that are easier for our assembly line to understand. This means creating a drawing more like a step by step instructions. This means breaking up the complicated assembly into separate stages and we are doing this by creating simplified reps for each stage of assembly. However, we need an easy way to assign BOM balloons to each of the simplified rep views. Currently we assign a separate BOM table to each view and fix the index numbers to the same index number in the master rep BOM. This is very time consuming and there is a risk of mistakes.

I had two ideas as a solution, but I cannot get either to work.

Idea 1: Create BOM table with multiple &rpt.qty columns with each column assigned to a different stage. This works well because it shows all of the stages and the quantity of pieces at each, however, we cannot attach BOM balloons to any views because of the following error: "BOM Balloons are not supported for regions with multiple models."

Idea 2: Create a component parameter for each component in the assembly and call out this parameter in a custom balloon in each of the simp rep boms. I have been able to do this, but it seems very time consuming still because I have to individually create the parameter with each component. Is there a way that I can create a component parameter for all of my components and the then edit the parameter in the model tree.

Can someone help me find a work around?

2D Drawing

C

Chris3

21-Topaz I

First, if you haven't already, I would suggest you upvote this idea: Allow BOM Ballons from Master Rep Repeat Region to be displayed on Simplified Reps

We have solved this problem a couple of ways. One is what you mentioned - fixing the index on multiple regions.

The second is to change your balloons to be custom balloons. We have balloons that instead of calling out the find number call out the actual part number.

The third solution is to exploit a big in Creo that has been around for multiple releases. Hopefully they don't fix this, but no guarantees going forward. Creo won't let you move a balloon from a master rep view to a simplified rep view using the move item to view command. It will give you the error you mentioned. However, if you right click and choose "Edit attachment" and the change the selection from change ref to same ref, it will move the balloon to a view with a different rep. It can be a little tricky. The way it works is if you hover over the same line, surface, etc that the balloon is currently pointing to on your master view then the balloon will jump and point to the same line, surface, etc on any over view.

You might also want to look into Pro/Process. Its called "Process Plan" or "Process Planning" now. It's a part of the Advanced Assembly Extension.

T

tvasina-2

1-Visitor

Hello all, unfortunately the third solution does not already work. Seems that they have fixed the bug

C

Chris3

21-Topaz I

What version and datecode of Creo are you using? I just tried this in Creo 4 and it still works. If they haven't fixed it in Creo 4 I find it hard to believe they fixed it somewhere else.

D

dgschaefer

21-Topaz II

As Christopher said, If you have Advanced Assembly, you want to look at the Process Planning functionality. It is made for this exact scenario and makes this quite easy.

I'd look at it first, if you have it it will save you a lot of effort.

V

vwilliams

7-Bedrock

@dgschaefer wrote:
As Christopher said, If you have Advanced Assembly, you want to look at the Process Planning functionality. It is made for this exact scenario and makes this quite easy.

I'd look at it first, if you have it it will save you a lot of effort.

I realize this response comes 10 years later, but in PTC enhancement request years, this is fast... apparently.

Aside from needing the Advanced Assembly license (we have one license we have to share and we get scolded by IT if we use it too much), my attempt to use Process Plan did not solve the problem. It still creates a separate BOM for each step and restarts BOM find numbers at 1 for each step in the process. I still have to fix the index in each step's BOM if I want continuous find numbers for the entire assembly.

Honestly, I don't see what value the Process Plan brought to my workflow. I had to create and manage an addtional assembly referencing my actual assembly, and work to build the steps. In the end, I think the simplified reps were faster and easier, and the Process Plan didn't add anything I didn't have before in the main assembly with simplified reps. The dream of easy BOM updates and parametric item balloons is still out of reach all these years later.

Creo 8.0.10.0

H

hkenyon

1-Visitor

Hi Cameron,

It's a year later but this might still help! I've struggled with this for a while now and I think I've figured out a workaround. We have the same problem about trying to break down our assembly drawings into stages for instructive purposes and simplified reps just don't have the right options. I've ended up creating layers and hiding in the view then saving status to do it. This will allow you to hide components without creating a simplified rep. You can also select entire groups and patterns to hide rather than having to select each individual component. The BOM balloons can then be created by view (and it will automatically exclude the parts that are hidden). I've so far found it hasn't caused any problems but it's still early days!

My solution is as follows:

In your assembly, instead of creating a simplified rep, create a new layer.
1. In layer tree, right click > new layer.
2. Include all components you will want to hide in this layer. At this point you can change the layer tree back to model tree to select things from there (including patterns and groups).
3. Click OK
Now open the corresponding drawing and place a view.
Select the Layer Tree window and ensure the view you have placed is selected. You can use the select tool in the layer tree as well.
Scroll down to the layer and right click > hide. This should hide the components you selected earlier in that view only.
Right click ‘Layers’ > Save status.
Now you can place your BOM table and create balloons by view. This should only create balloons on the visible components.

Hope that helps! Let me know if you find any issues as I've only just started using this method.

Cheers,

Hannah

J

JavierL

12-Amethyst

what solution did you implement?

I am running into the same problem and the edit attachment "bug" fix no longer works in Creo 6 so I am needing to find another solution

C

Chris3

21-Topaz I

As of now the only solutions are:

1. Keep using multiple repeat regions and fix the indexes.

2. Use component parameters. I haven't tried this myself but from what I read it works although complex to setup.

3. This may not work for your company - but I am now using custom balloons that just have the real part number rather than a find number.

W

wbottis

14-Alexandrite

I believe another ridiculous workaround is to insert the view (using master rep). Then, "blank" the components that are not relevant using the 'component display' > "blank components by view". Not having Creo active to confirm (currently, Creo 5 is not responding...), you should be able to add your BOM table and show balloons. I don't think balloons will be assigned to those components that have been blanked. I like to have my find numbers correlate to the order that the parts and sub-assemblies appear in my model tree (e.g. find number 1 is the first item in my model tree). Repeat this process on each sheet if you have a large assembly.

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