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Midplanes in assemblies

22 REPLIES 22
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Message 1 of 23
chipwitch2
3389 Views, 22 Replies

Midplanes in assemblies

I'm a little confused.  After reading the documentation for IV 2013, I'm not sure if it's possible to create a midplane between parallel faces of two different parts or not.  I've tried using the workplane buttons in both the 3D Model and the Assembly tabs with no joy.

 

Can someone please clarify?

 

Thank you.

Product Design Suite 2013 Ultimate
Windows 7 64-bit
Intel Core 2 Quad Q9300 2.5GHz
8 GB RAM
Nvidia GeForce 8800 GT
22 REPLIES 22
Message 2 of 23
blair
in reply to: chipwitch2

You would need to use a parameter

 

If the one plane is constrained to another work plane, you should be able to use the paramter ID / 2 as your mid distane.

 

Work-Plane 2 is contrained from Work-Plane 1 by contraint "d26". You should then be able to us "d26/2" for your distance when you create your mid Work-Plane


Inventor 2020, In-Cad, Simulation Mechanical

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Delta Tau Chi ΔΤΧ

Message 3 of 23
t_stramr
in reply to: chipwitch2

Hi,

 

Inventor 2013 does not provide midplane constraint. Workaround is to create Mate assy constraint between two planar faces. Then use half of constraint modifier(distance) as a parameter when creating new work plane defined by perpedicular distance form a plane.

 

Hope this helps.

 

Robert

Message 4 of 23
blair
in reply to: t_stramr

Correction, I should  have used "Offset" rather than constrained, but the same parameter methodology will work.


Inventor 2020, In-Cad, Simulation Mechanical

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Message 5 of 23
karthur1
in reply to: t_stramr

I know this is an old post, but I was trying to create a midplane at the assy level and could not do it.

 

Robert, you say that this is not supported in Inventor 2013.  You say that like it is supported in a different version.  I just tried it in 2014 and it does not work in it either (unless I am missing something).  I was doing something similar to what you suggested, but that requires the offset to be manually adjusted if something changes.  I wan the midplane to be stay in the middle then things move in the assy.

 

There is an "accepted" IdeaStation thread that addresses this. Hopefully, this will be addressed in a soon-to-be-released version.

Message 6 of 23
JavaLodge
in reply to: karthur1

I believe he wanted it to mean that it was not supported in 2013, but may be in future versions precisely because of the Idea Station thread you mentioned.  

 

The method he was metioning goes like this:

 

Make a parameter to reflect the distance apart you want your parts to be, say 'width' or something like that.

When you constrain those parts together, use an offset contraint and when you type in a value for the distance of offset, type in the parameter name you created.

Now make an offset plane from one of the faces you contrained earlier, and make the offset equal to half the distance.  You can use parameter names in equations, so you can just type width/2 and the plane will always remain halfway between those two parts.

 

You have to remember to update the parameter and not the contraint if you want to change the distance between them though.

Hope this helps.  See the attachment for more clarification.

____________________________________________________________
Slow is good and good is fast.
Message 7 of 23
karthur1
in reply to: JavaLodge

Yes, I totally get how he was saying to do it.  Its just that I did not want to have to use parameters (I would forget to change it later).  The way that I did it was to use an assembly sketch with a line between the two surfaces.  I put a point in the middle of the line and dimensioned to the point.  Next, I created a plane and offset the plane with the driven parameter to the center point.

 

Now, when the parts move, the mid plane "automatically" adjust to be between them.  See my video here.

 

Thanks,

Kirk

Message 8 of 23
JavaLodge
in reply to: karthur1

Ah, that's neat!  I'll have to remember to do that the next time I need this.  I apoligize if I sounded condescending or anything.  I agree with you that this kind of workaround is a bit silly, and I really hope that Autodesk would add this feature because I would use it every day.

____________________________________________________________
Slow is good and good is fast.
Message 9 of 23
blair
in reply to: karthur1

This would be a tough one to automate in an assembly. Lines and edges all have mid-points that you can construct to. I don't know how you could get an automatic mid-plane on a assembly. Short of constructing a "Bounding Box" around the assembly and then having a work plane on the mid-point of the edges. An adaptive box, but then as soon as you add a component to the edge of the IAM it would not be included in the adaptive box.

Inventor 2020, In-Cad, Simulation Mechanical

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Message 10 of 23
blair
in reply to: blair

I guess, that I am thinking that as you build a IAM and add parts you could get a automated center mid-plane. I deal to much with vehicles and build everything off the center mid-plane.

Inventor 2020, In-Cad, Simulation Mechanical

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Message 11 of 23
riveter1000
in reply to: karthur1

I am using this sketch based midplane technique in an assembly. It works in the master position representation, but when I switch to another position representation, the sketch does not update. How can I keep the sketch associativity?

 


@karthur1 wrote:

Yes, I totally get how he was saying to do it.  Its just that I did not want to have to use parameters (I would forget to change it later).  The way that I did it was to use an assembly sketch with a line between the two surfaces.  I put a point in the middle of the line and dimensioned to the point.  Next, I created a plane and offset the plane with the driven parameter to the center point.

 

Now, when the parts move, the mid plane "automatically" adjust to be between them.  See my video here.

 

Thanks,

Kirk


 

 

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M
Message 12 of 23
karthur1
in reply to: riveter1000

Does it update if you click rebuild all after you change the PR?

 

What version are you using?  In 2015, we now have assembly midplanes.

 

2014-06-11_1140.png

 

Kirk

 

 

Message 13 of 23
riveter1000
in reply to: karthur1

It does not update if I hit rebuild. Here's a screenshot showing sketch which stays attached in the Master representation but detatches in the other represenatation. I am on Inventor 2014 and am due to get Inventor 2015 later this month. That will be a welcome addition.

 

Image 001.png

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M
Message 14 of 23
riveter1000
in reply to: riveter1000

The problem file attached is attached.

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M
Message 15 of 23
karthur1
in reply to: riveter1000

It does not like the positional rep.  I can stay in the Master PR and adjust the  offset between the frames, then rebuild all and it works correctly.

 

Using the new midplane works much sweeter, but that does not really help you much till you get 2015 going.

 

Here is a video of your assembly with the midplane.

 

Kirk

Message 16 of 23
riveter1000
in reply to: karthur1

That's pretty sweet. I should have Inventor 2015 in a few weeks. I'll be using that feature a lot.

Thanks much for looking at it for me.

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M
Message 17 of 23
SBix26
in reply to: riveter1000

Since an assembly workplane is basically a component, it can be constrained using the symmetry constraint (new in 2014).  Disclaimer: I have not tried this on your posted assembly.

Sam B
Inventor 2012 Certified Professional

Inventor Professional 2015 Update 1
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

Message 18 of 23
riveter1000
in reply to: SBix26


@sbixler wrote:

Since an assembly workplane is basically a component, it can be constrained using the symmetry constraint (new in 2014).  Disclaimer: I have not tried this on your posted assembly.

Sam B
Inventor 2012 Certified Professional

 

It does not work for me in Inventor 2014. It just puts the plane out in space by all by itself.

 

Image 005.png

 

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M
Message 19 of 23
karthur1
in reply to: riveter1000

Another way to do this is to drive the offset distance for the plane with a dimension.  Here is a video of that if you are not fimilar with this technique.

 

I used the "d53" dimension which is the parameter for the "Adjust Me then Rebuild" constraint.  When you change this, then the offset distance for the workplane changes.

 

Kirk

Message 20 of 23
riveter1000
in reply to: karthur1


@karthur1 wrote:

Another way to do this is to drive the offset distance for the plane with a dimension.  Here is a video of that if you are not fimilar with this technique.

 

I used the "d53" dimension which is the parameter for the "Adjust Me then Rebuild" constraint.  When you change this, then the offset distance for the workplane changes.

 

Kirk


Thanks for that video Kirk. The method works great.

Mark

Inventor Professional 2015 SP1

System Specs:
Dell Precision M6800
CPU Intel I7-4600M
RAM 16 GB
Graphics Nvidia Quadro K5100M

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