derived parts & arrays

[cadman777]

Can someone tell me if there's a way to do this:

I have a derived part that's identical to its parent part, except that it's mirrored.

I want to do an associated array of fasteners in the holes that were arrayed in the parent part, and show-up in the derived part.

I can't get the assocated array to function in the derived part.

Is there a way to make this  derived part act like its parent part so I can accomplish this associated array in the derived part?

[SBix26]

My approach is to do the mirror operation in the layout (mirror entire solid to a new solid), then you can do the array there and choose which solid it applies to (in fact, even though a hole can go through multiple solids, a pattern of that same hole can only apply to one solid).  Then derive to individual parts.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 1
Windows XP Pro 32-bit, SP3
HP EliteBook 8730w; 4 GB RAM; Core™ 2 Duo T9400 2.53 GHz; Quadro FX2700M
SpaceExplorer/SpaceNavigator NB, driver 3.7.18
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[cadman777]

Thanks Sam.
The first part I already do.

But I don't understand what you're saying in the 2nd part (in the parentheses).

Would you send an example or link me to a pdf showing the process-flow?

[SBix26]

I don't have anything immediately at hand to illustrate.  But I'll try to explain with a bit more detail.

To create right/left hand parts, I start with a layout, which is a part file in which I create the two solids.  I then derive these solids into two separate parts.

1. New .ipt file (e.g. Layout.ipt)
2. Create one of the parts (e.g. right hand) with a logical relationship to the origin.  This solid contains all the common features of the right & left hand parts.
3. Using the Mirror tool, choose Mirror a solid and New Solid and select the appropriate mirror plane; now there are two solids in the file, one the mirror of the other.
4. Continue to add features to the individual solids that are distinct from each other; if you discover that you need additonal common features, just pull the EOP marker above the Mirror feature and add them there, then pull the EOP back to the bottom.
5. When complete, use the Make Components or Make Part tools to derive the two solids into two individual part files (e.g. Right Hand.ipt & Left Hand.ipt); in these files set Materials, Appearances, part numbers, descriptions, etc.)
6. Add Right Hand & Left Hand to your assembly.  If the layout's origin point was chosen to correspond with the assembly's origin, they can both be grounded at the origin (not in the case of moving parts, of course).
7. Any changes are made in the Layout.ipt file, and an update to the assembly immediately makes those changes visible.

As for the bit I put in parentheses in my previous message, that's just mentioning a current limitation of multi-body solids.  Some tools can apply to multiple solids, some cannot.  Holes can, patterns cannot.  So, even though I can put a hole through three solids in one feature, if I want to pattern that hole through the same three solids, I will have to create three separate pattern features, one for each solid.  Pretty annoying, and makes a cluttered feature browser, but at least it's possible.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 1
Windows XP Pro 32-bit, SP3
HP EliteBook 8730w; 4 GB RAM; Core™ 2 Duo T9400 2.53 GHz; Quadro FX2700M
SpaceExplorer/SpaceNavigator NB, driver 3.7.18
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[cadman777]

Sam,

Thanks for the good explanation.

I do use multi-body parts like that.

I also do the 'short-cut' method of creating all the left-hand parts in the multi-body part (your "Layout ipt"), and then I mirror them into separate ipt's in the iam file. That leaves my multi-body part less large, b/c it tends to slow down the machine when the multi-body ipt's get big.

Either way, there's those "annoyances" that always "clutter-up" the browser and create massive overhead in the model, as you mentioned.

Thanks again for the good explanation.