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Drawings for multi-config assemblies

conrat

New member
Hi all,



I work for a small manufacturing firm that makes various sheet metal
products. We make a line of door assemblies, which depending on
what a client needs, change parts and configurations based on their
needs.



The problem we run into is when those parts change, are supressed, or
get swapped out for other parts. Sometimes dimensions do not show
up or change to a mageneta color (lost references). Other times,
views do not appear correctly due to a size change. Other times,
notes appear to overlap or leaders disappear.



We use Pro/Program and drawing states exclusively to try and control
these issues. However, because of the number of "states" required
to get the drawing to display correctly, it is quite cumbersome to
create a state for ALL possible configurations.



Does anyone know where I might find information on this sort of
thing? Controlling multi-configurations using the same assembly
on drawings?



We don't have a problem creating drawings from scratch. It is the
maintenance of the changing configurations that is throwing mokey
wrench after monkey wrench into our work.



Thanks in advance,

Jim
 

Isair

New member
Hi Jim, again me
It seams that we have similar problems with ours variant contractions

I don't believe there is a full solutions to this problem but if anyone knows better solutions, or have better idea pleas post it here.
So here is how I solved this kind of situations, well not all there is still manually work about it but it helps.


First of all if you know all versions of construction the it is a little bit easier, because then you know yours bigger, and yours smaller outer dimensions. But then I suppose this isn't case here.


First what I have created ware construction planes, points, and axis, their dimension if they have some connected to relations. This way when I create dimension in drawings I associate dimensions to points, datums and axis rather to associated them to geometry.


Second, I have created construction curves where I was unable to create datums, points, (because of complex geometry) and then using show dimensions I display their dimensions in drawing. Also all dimensions of this curves ware connected to relations and parameters.


This way I have control when and where some dimensions would be displayed, and to ensure myself that dimensions don't loss reference because of geometry changes (sometimes when geometry changes this edges, surfaces, points where dimensions were associated lose their previous ID and get new one so dimensions loose their references - why this happens I don't know).


Also all assemblies should have their right simp reps in drawings. I have also used to created dummy parts and asm for purpose of creating detail views, sections and repeat regions (for bom balloons). All that dummy parts and asm have got relations, and parameters.


And in the end while in drawing create drawing program for executing particular views, or showing particular dimensions, for creating detailed views etc. But be careful because drawing program recognize only parameter that was used in relations, not this ones that are in parameter of parts or asm. In other words all parameter you wont to use in drawing program you must set in relations of asm or part which you want to use in drawing. Also be careful using multiply models in drawing.


Hope it will help, if you have any questions about it just ask and I will answer if I know.
Also if anyone else knows other method please post here!
 

conrat

New member
We have been controlling missing references by creating multiple view
of the same section, with different things dimensioned on each.
Then, depending on which view is the "correct" view, we use the drawing
program to move them onto the drawing sheet. If it is the wrong
view, we move them off of the page border, so they do not print.



This does make for some double work, but it does work somewhat.
It is just extremely cumbersome to create the same section multiple
times and then write relations to pull them in.



It would be nice if Pro/E would just delete the dimension if it is not needed.



I will share any tips I come up with.



Thanks,

Jim
 

Ascorti

New member
I cannot say that I have any experience with Pro/Program but I can tell you how we handled a similar situation with large assemblies. The company I used to work for had a base model assembly with multiple options. The variations were originally handle with a family table but this soon became quite cumbersome due to the size of the table. We went to using simplified reps and then setting the rep we wanted in a drawing and adding the related view. We didn't have trouble with dimensions or other items related to each rep that I can think of off hand. The one caution I have is that you make sure all the reps are in session and the drawing rep is set to "master" to prevent loss of data. Pro/E will caution you when you are using simplified reps and trying to save a drawing.


I hope this helps.
 

conrat

New member
Ascorti,



I am new to simplified reps, but plan to look into them in great
detail. I will post back any successes/problems I run into.



Thanks,

Jim
 

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