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Assembly Parametrics ???

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I know that you can use parametrics in a part, but in an assembly?

 

I want to design a model one time.

Then, if the need arises for a 2nd model, almost identical, is it possible to set up parametrics, so that I wouldn't have to create a whole 2nd model?

 

Just SAVE AS, & modify the dimensions in the 2nd model.

 

For example, in the 1st model, PART A should be offset from the edge of PART B by 4 inches. If I were to change the overall length of PART B in the 2nd model, PART A should still be offset by 4 inches.

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shift1313

Yes. You can also drive models with an excel spreadsheet. I haven't done this in Inventor in many years. There are also a lot of functionality built into intelligent parts. Do you have a more specific example or sample file?

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... Do you have a more specific example or sample file?

 

 

Here is a PDF of my assembly.

Very lame, not extravagant, but enough (I hope) to get my point across.

ASSEMBLY 1.pdf

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shift1313

makes sense. How are these parts attached to each other? There are several ways this could be handled. If you do this at the part level(or even the assembly level working in-context) you just simply dimension the channel to the edge of your plate. The dimensions will handle it and you don't need any special work around or anything like that. Further than that if you make use of symmetry you can dimension just one side and then mirror it.

 

If you want to use named parameters you will find those on the "Manage" tab. You could also get really fancy and make the rails intelligent parts that automatically insert and scale. Really depends on how much time you want to put in on the front end.

 

iPart is the table driven part if you think you will have dozens or more of these "configurations".

 

I attached a file here that is all a single part. If you go to the "Manage" tab and select Parameters there are 3 named parameters. Plate_Height, Plate_Width and Edge_Space. If you change the 96" Plate_width you will see that the Channels move with it. If you want to you can "Make Components" from a file that contains multiple bodies. When you do this you have a button called "Include Parameters" and you can bring in specific dimensions you want in the assembly. I haven't tried it on this example but might be worth a look.

Adjustable Plate - Copy.zip

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Shift1313 -

 

Thank you for the very detailed response.

I am not sure if I fully understand, but I will follow your instructions, & see if I can get it to do as you said.

 

I'll post here, as to whether I was able to duplicate your example or not.

 

Thanks, again.

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Well, I downloaded the zip file, extracted it & attempted to open it.

I got this error message instead.

 

 

Anyone have any idea as to how to get around this "newer version" issue to get the .ipt to open? (BTW, I am running Inventor Pro 2015.)

NewerVersion.png

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-(Duplicate post.)

Edited by vertical horizons
Duplicate post.

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"... I attached a file here that is all a single part. If you go to the "Manage" tab and select Parameters there are 3 named parameters. Plate_Height, Plate_Width and Edge_Space. If you change the 96" Plate_width you will see that the Channels move with it. If you want to you can "Make Components" from a file that contains multiple bodies. When you do this you have a button called "Include Parameters" and you can bring in specific dimensions you want in the assembly. I haven't tried it on this example but might be worth a look."

 

 

The reason that I was asking about doing the parametrics as an assembly, instead as a part, is because I would want for all of the components to be identified in a Bill of Materials. If I were to do this as a part (all 3 pieces, the 96" plate & the 2 channels, as one), even though it might look correct, wouldn't it list it as just one part?

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sorry for the delay. I don't know of any way you can open the 2017 file in 2015 and keep all the parametrics in place.

 

As for the part vs assembly. I can't recall off the top of my head but i seem to recall you can make a BOM with a single part file and multiple bodies.

 

Either way, if you just do this as an assembly all you need to do is make sure you either have an offset plane in the main plate part(the 96" wide part) that you can align with in the assembly. This way you can control everything from that single part if needed. Or just make sure when you put the parts together that you specify 4" from the end face and it will update automatically. There is a lot more to it and unfortunately i don't have the time at the moment to make you a video or something. Hopefully someone else is able to chime in that has 2015 installed and provide you with some files you can open.

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Shift1313 -

 

Sorry. I didn't realize that you were running IV 2017.

That explains the error message. Iii

 

I will tinker with it a little more, & if I find a solution, I'll post it here.

 

BTW, I thought of a good use for parametrics ...

F&D heads use a formula to determine their dimensions.

 

I could see creating JUST ONE F&D head, using parametrics, then being able to quickly create others, as needed, by simply plugging in a different diameter.

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shift1313
Shift1313 -

 

Sorry. I didn't realize that you were running IV 2017.

That explains the error message. Iii

 

I will tinker with it a little more, & if I find a solution, I'll post it here.

 

BTW, I thought of a good use for parametrics ...

F&D heads use a formula to determine their dimensions.

 

I could see creating JUST ONE F&D head, using parametrics, then being able to quickly create others, as needed, by simply plugging in a different diameter.

 

I have used table driven files and equation driven file for lots of different designs. Once you start playing around with it you can find all kinds of things. The tricky part is modeling and setting up a file that will update for a wide variety of changes. It comes down to be careful with how you setup sketches and features.

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Ok, I finally figured out how to do it.

 

 

I went into my Excel sheet, & changed Clearance_Check's column B to read "(Length/2)-6.75". (Whatever the length is, divided by 2, then subtract 6.75". [6.75" = 4" clearance that I want to have, plus 2.75", which is the width of the channel].)

 

 

I constrained each of the 2 channels to the midplane of the 96" panel, & for the offset distance, under "List Parameters", I selected Clearance_Check.

 

 

Now, whenever I change the Excel sheet length, not only does the 96" panel's length change, each channel moves accordingly.

 

 

Works like a charm.

 

 

BTW, I probably could have chosen the other side of each channel, & wrote a smaller formula (Length/2)-4, but I'm pretty happy with the results.

 

 

Shift1313,

Thanks for all of your input.

I appreciate it.

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