New Part could use mating part as background

Hi,
I need to draw a new part that fits together with an existing part. Can I use the existing part as background/references whilst I draw the new part?
tia,
Matthew Rutherford.
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Of course, that's what parametric design means.
Create an assembly, assemble the existing part, then create the new part within the assembly using the existing part for your references.
If later you want the parts to be independent, i.e. no longer parametric, then open the new part, and redefine the features, deleting the external references.
Dave
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Thanks for the advice.
After I created the new part in the assembly, I realised I had failed to select a reference. I can sure redefine the part/delete its (sketch) references OK, but how do I go back to the 1st part in the assy and select the missing reference?
Regards Matthew

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part?
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Not sure what you mean. What is driving the assembly; what would you reference in the first part?
Or, are you asking how to reference geometry that exists in the first part? A really simple example; a pump housing that will interface with a gearbox drive pad.... In an assembly that contains the gearbox case, create the housing part constraining it to the gearbox or default datums. Activate the housing part. Select the mating gearbox face and Edit / Copy (or any of several other methods of creating local copies of external geometry).
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: Thanks for the advice. : : After I created the new part in the assembly, I realised I had failed to : select a reference. I can sure redefine the part/delete its (sketch) : references OK, but how do I go back to the 1st part in the assy and select : the missing reference? : I have to agree with Jeff. I'm not sure where you are in this process, where you are stuck or how you got there. Many people who come here seem shy about telling us what they did. Maybe they are just so lost that they don't know. But it helps those of us who know these problems to have kind of a process sheet that tells us where you got stuck and how you got there. That means describing what you did and where you are in some detail. I realize that the newsgroup culture pushes against elaboration, toward the brief and breezy, but we really need to be looking over your shoulder, we need pictures in this text NG, but all we have is your description. The vaguer your description, the more we have to guess. I'm guessing that the problem, whatever it is, began with the assembly. I'm also guessing that you could be talking about problems with creating new references in sketcher. I don't want to guess and give needless, scattershot advice. I'm lazy, I want you to lead me by the hand. I really am quite simple minded, I miss the pictures and your words have to make up for this deficiency or you could send me a screen shot. I need something. Yeah, I know I talk too much. But you guys don't have to make up for it by talking too little!!! In the words of the immortal "Jerry McGuire": "Help me help you."
David Janes
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OK.
To test what was going on, I
created a simple 'cuboid' part, then made hole in one of its faces, ie a blind cut with a five-sided section (as it happens).
I then created an assembly, and assembled the cuboid part into it.
I then created a new part within the assembly, the idea being that this I would fit into the hole in a certain way 9made up on the fly). Crucially, though, I would resize the cuboid part, and wanted to check that the 'insert' part resized as I expected, all fine and dandy.
So, when I created a new part within the assembly, I selected as references the inside surfaces of the cuboid part's hole.
Problem was, when I resized the cuboid part, the insert part resized not how I wanted it to.
I realised I needed, within sketcher, to grab a few new references from the surfaces of the cuboid's hole to make the inserted part behave as I wanted. However, when I 'redefined' the insert part in sketcher and listed the references, it said 'cuboid part:surface 1' etc etc, and I could delete any references easily enough. I couldn't though see how to grab a new reference from the cuboid for sketcher.
That was my problem!

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Did you regenerate the child part after modifying the parent?
I'm not sure I fully understand the regen process (actually I'm sure I have questions about it), but the surest way I know of to make sure everything is up to date is to Custom Regenerate the assembly; twice. Are there any config options that govern such things?
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I did a regenerate / automatic. The insert definately changed shape! Just not according to my intent!

have
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Ok, apparently an underconstrained shape, so to go back to...

I might be missing something. Once back in sketch mode; menu Sketch / References... (I'm assuming you were there, "listed the references" can mean a number of things), pick the additional references.
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: OK. : : To test what was going on, I : : created a simple 'cuboid' part, then made hole in one of its faces, ie a : blind cut with a five-sided section (as it happens). : : I then created an assembly, and assembled the cuboid part into it. : : I then created a new part within the assembly, the idea being that this I : would fit into the hole in a certain way 9made up on the fly). Crucially, : though, I would resize the cuboid part, and wanted to check that the : 'insert' part resized as I expected, all fine and dandy. : : So, when I created a new part within the assembly, I selected as references : the inside surfaces of the cuboid part's hole. : : Problem was, when I resized the cuboid part, the insert part resized not how : I wanted it to.
How did you want it to locate or resize? If, as I suspect, you wanted the associated second part feature to stay 'centered' on the five sided hole, then don't pick the sides for references. Use datums for your references. But for the hole geometry, create the smaller hole by offsetting the hole edges. That way you get the location and the size. You could also create additional reference geometry in the base part which could be used as a reference, such as a construction circle tangent to the sides and an axis point that could be referenced by your associated second part feature. These techniqes let you use the base parts location references with out constraining the size of the second part's geometry. There are additional techniques that can be suggested if the above doesn't quite get at the problem.
BTW, thanks for the more complete description. To a greater extent, it lets me "look over your shoulder".
David Janes
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: Hi, : : I need to draw a new part that fits together with an existing part. Can I : use the existing part as background/references whilst I draw the new part? : Good question, ought to be in a Pro/e FAQ (even though it hasn't been asked very often).
There's suite of techniques that is roughly called top down design or, in the case of that suggested by dakeb, assembly modelling. Another involves also working in assembly to create the common featues in both at the same time with assembly cuts. There is a basic explanation of the technique in the Help documentation in the Assembly and Welding functional area, Pro/ASSEMBLY module, the section on Assembly Operation, Working with Subtractive Assembly Features.
Further techniques are described in the Advanced Assembly module, the section on Data Sharing. The techniques include Inheritance features and Copy Geometry. While the Help documentation is not a tutorial, there is some 'How to...' stuff as well as the overview and rationale behind the techniques.
David Janes
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The easiest way I find is to use the copy geometry feature: insert > shared data > copy geometry from other model
Open the other model, use the default coordinate system then you know they will align in an assembly.
Choose the type of geometry you wish to copy and then pick the elements which represent the interface.
Choose to make it dependent or independent.
These can then be use to construct the new model.
Sean
WF2
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