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New to Creo - Parameter Roll-Up in Assemblies

mwick
2-Guest

New to Creo - Parameter Roll-Up in Assemblies

Hello,

I am new to Creo and I am guessing this is a basic thing. I have created a Parameter in my Part and Sheetmetal templates for Total Estimated Weight. I have also created that same Parameter in my Assembly Template. I have relations in the Part and Sheetmetal files that allow for adding weight manually if these are purchased parts, or welded, to had weld weight. In my assembly I want to total all the "child" weights into the "parent" Total Estimate Weight Parameter, but I am not sure how to write a relation to do that. Can someone help?

Thanks,

Mike

14 REPLIES 14
huggre
1-Newbie
(To:mwick)

Hi

Creo automatically calculates weight and assign this value to a system parameter if you set the mass_property_calculate = automatic in your config.pro.

The name for this parameter is pro_mp_mass

If you want to assign this value to your own parameter you can simply add the following relation to your start part.

weight = pro_mp_mass

Note that these calculation are based on the volume and density of each individual part in your assembly and not based on any weight parameter you may have added to the individual parts.

Hugo

mwick
2-Guest
(To:huggre)

Hugo,

That is my issue, I need to be able to calculate the total weight based on the user defiend parameters of the individual parts. Not all the parts in my assemblies have an acurate density or even a model. I wish I could rely on that, but unfortunately that is not always the case.

Thanks though

Mike

huggre
1-Newbie
(To:mwick)

Mike

Try this:

1. Create a real parameter (weight) in your model and specify the correct weight

2. Add the folowing relations to the part

mp_density=weight/mp_volume(“”)

/* The relation will now change the density according to your specified weight

/* This is an old relation we used previously and has not been tested with creo

Hugo

mwick
2-Guest
(To:huggre)

Hugo,

The problem is that sometimes I don't even have a model/solid just an empty part say for fluids. I have the weight of the fluid that is in the assembly but not a solid model. Others things that I have run into is "mixed" material vendor parts. I have a single solid for a mirror assembly that is made out of steel, glass, rubber, and plastic, and a weight. I that case the relation you have suggested would work, but I already have a parameter for vendor weight, which rolls up into a Total Estimate Weight parameter on the part.

Mike

huggre
1-Newbie
(To:mwick)

Mike

For items you want to include in your assembly but does not have solid geom. you should look into "bulk item"

This is a special kind of part in Creo

Hugo

mwick
2-Guest
(To:huggre)

Hugo,

So is there no way in a relation to "roll-up " or add together all the values of a parameter in children parts into a parameter in the parent assembly? Let's forget it is a weight, how about if all the children have a cost parameter that is manually entered, can there be a relation that adds up all the child costs into a parent cost parameter?

Mike

dschenken
21-Topaz I
(To:mwick)

This capacity is carried on drawings in the form of Tables and Repeat Regions. There are report variables that can do the summation.

http://communities.ptc.com/thread/39379

Good or bad, there isn't a direct method to do this in the model, but since it has to get printed sometime, it can show up there.

huggre
1-Newbie
(To:mwick)

Mike

Even if this is not an out-of-the box function in Creo it should be pretty straight forward to create this function using Jlink or VBA.

Hugo

jsarkar
1-Newbie
(To:mwick)

I had similar kind of issues, however I have overwrite the mass properties by FIle> prepare>model properties>change select geometry and parameters. Set the mass with all additonal weight.

Then I go to mass property analysis and select assgined so that you can get total weight including your addtional weight. (Note assigned is only available if you overwrite mass properties)

Hope it might solve your problem

Regards,

Jayanta Sarkar

gkoch
1-Newbie
(To:mwick)

As mentioned by others:

1. There is no functionality in the model to summarize parameter values (of course you can write relations in the assemblies that compute sums of component parameters, but it would require to always adapt the relations to the assembly structure).

2. Summarizing is available only within report tables in drawings.

In addition to that:

1. I believe there is also some summarizing ability for customized BOM Info output, but this will only be generated when outputting info (to a window or text file) and it is not available inside the model

2. Going back to the original example of summarizing masses: For parts where the density is not specified, there is the possibility to define alternate mass properties: This allows to simply specify the mass (and other properties) as a typed in value for system parameters, e.g. PRO_MP_ALT_MASS. Whether to use calculated or specified properties, can be set by the mass properties parameter PRO_MP_SOURCE and/or recently by the config option mp_analysis_default_source, see CS154371: How to control the default mass property calculation method in the Analysis > Model > Mass Properties dialog box in Creo Elements/Pro 5.0 (https://www.ptc.com/appserver/cs/view/solution.jsp?n=CS154371)

hi i am also facing same issue do you find any solution for it.......in this communication there is no conclusion please help me on this

 

Regards,

Anil

Dale_Rosema
22-Sapphire I
(To:huggre)

Is there a way to just view the weight value without putting it on a drawing? Or do you need to place is somewhere on the assembly drawing to see it?

I have added the parameters to the Model Tree as additional columns. That way you can see all the values from the parts that make up the assembly as well.

mwick
2-Guest
(To:mwick)

Thank you all for the information. I have come up with some relations and parameter mixes to be able to roll up the weight that is needed. By using the Hugo's suggestion of changing the density to affect the mass and an additional process change I can roll up the mass of parts into the actual mass of the assembly quite effectively.

Thank you all again.

Parameters:

TOTAL_EST_WT=(Real) - This is the parameter the drawing reads

EST_PURCH_WT= (Real) - use if purchase weight is known and model is "estimated" - aka non-exact solid

WELD_WT=(Real) - use this if weld weight is known - otherwise we have setup ProWeld to add to mass

------------------------------------------------------------

Relations:

/*Calculating Weight

IF EST_PURCH_WT!=0
mp_density=EST_PURCH_WT/mp_volume("")
ENDIF

IF EST_PURCH_WT!=0
TOTAL_EST_WT=EST_PURCH_WT
ENDIF

IF WELD_WT!=0
TOTAL_EST_WT=pro_mp_mass+WELD_WT
ENDIF

IF WELD_WT==0 & EST_PURCH_WT==0
TOTAL_EST_WT=pro_mp_mass
ENDIF

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