automatic part generation/modification?

Hi,
I am quite new to Pro/E Wildfire (about 3 months use) and have the following
question:
Quite often I need to create a set of maybe 8 or 9 parts that follow a
standard layout. I have a set of dimensions and each part is made from some
or a combination of these dimensions. Instead of having to go through and
create/modify each part by hand, is there any way I can give ProE all these
dimensions and it will update all my parts in one go?
All the dimensions arrive in an Excel sheet and I'd be quite happy to write
some VB to put it in a format that Pro/E can understand.
Thanks for any ideas,
Scott
Reply to
scott
Loading thread data ...
Scott, Here are some key words to feed in to your favorite search engine (and try google.com looking in groups, comp.cad.pro-engineer):
family tables pro/program pro/layout configurator
If you're not in the mood to do it yourself, there are many consultants (ahem) who would be glad to help you set something up, and there are some 3rd party configurator applications available that might be worth looking into.
Paul
Reply to
Paul Rudolph
I'm not really in a position to buy more software, and if I'm not mistaken pro/program and pro/layout need to be purchased additionally? Are family tables really what I want? I thought I knew what they were about but perhaps not.
Let me give you an example of what I need to do that might help someone suggest a solution.
I'll use a roll of sellotape as an example.
I get in the dimensions in Excel (say overall diameter, thickness, width, length of tape etc). Then I create several parts (eg the cetnre spool, the winding of tape, protective cover etc). At the moment I need to go through each part and recalculate the dimensions based on the new ones I've just got in. It takes a long time, I have at least 10 parts with some quite complex relationships between the dimensions I get and the ones I need to use in Pro/E.
I guess the question I'm really asking is how do I use parameters in one part that are stored in/taken from another part/assembly? (and have them update automatically)
Thanks for the help,
Scott
Reply to
scott
I believe that the prior 'approved' method was to calculate the needed parameters in 'pro-layout' or use skeleton parts.
If I remember correctly, pro-layout was supposed to be able to pass the parameters and values to propogate downstream parts. I never tried to family table a pro-layout though...
Just my $0.02
scott wrote:
Reply to
Chris Gosnell
So, is there any way to access parameters in one part from another part? I don't have Pro/Layout, only the basic wildfire.
After much googling, Insert -> Shared Data -> Inheritance From Other Model seems like a good plan, but it's greyed out all the time...
Any ideas?
Cheers
Scott
Reply to
scott
I don't think so. With regards to Inheritance or insert/Shard Data/Copy geometry form other model..., you only get these features if you buy Advanced Assembly. Pro/Assembly-Performance included with Wildfire won't cut it. All you get is merge and cutout.
But...
One really wild-ass thing I can think of is to create a sketched datum feature (line or circle dia) whose length or diameter is driven by the parameter at part level. IF you created an assembly feature or a feature in the context of assembly, of the same type, would this be a way of communicating the numerical parameter value? Hmmm...
scott wrote:
Reply to
Chris Gosnell
I see where you're coming from, although that sounds a bit messy.
So, if I buy Advanced Assembly, I will be able to have one file called 'PARAMS.PRT' and have all my parameters in there. Then each real part I want to make I can inherit the parameters from PARAMS.PRT without having to enter them again. Then, when I need a new design, I can simply change the values in PARAMS.PRT, regen and the whole assembly will update automatically with the new dimensions? Is this correct?
Thanks
Scott
Reply to
scott
Again, I believe so. Either through Inheritance or through Pro/Layout which I believe is part of Advanced Assembly.
Good time to call your sales rep.
I am not so familiar with these options because from pro v19 through Pro 2001 (I don't know the build) I had these features, but my last build of 2001 and my current build of Wildfire don't have these 'options'. We are trying to negotiate with PTC to get these options added again, but I don't hold out much hope. (Yes, we are a long time user, and Foundation + packages is not equal to the old packages we had...
What is also interesting is that at one time I remember an article in Pro-E magazine (?) that explained the advantages of Insert/Copy geometry vs. Merge/Cutout. So, I get used to using Insert/Copy Geometry for a year or two, and now it is part of a module I don't have.
scott wrote:
Reply to
Chris Gosnell
Sorted it without needing to buy anything else.
In each part I have a list of parameters. Then in the assembly my relations set the values within the parts, eg:
var1:2 = var1 var2:2 = var2 var3:2 = var3
etc for each part.
Then, I can just change the values in the assembly and regen, and all my parts get updated automatically.
Scott
Reply to
scott
I have had some trouble with this in the past, wit ha family table, proe would sowmtimes pick up the wrong variables in a table.I would have to restart it then cheers Craig
Reply to
craig stevens
As Craig mentioned this migth give problems in family tables because ProE change the :2 (instance ID or something similar) depending on which instance you choose - then some of the variables fails
NielsC
Reply to
Niels Christensen
p-AdvancedBOM does most of what you want to do with it's bi-Directional Pro/E Ms-Excel interface. I would suggest you look at this.
formatting link
Dave
Reply to
Dave Bigelow

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