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Can't constrain curved face to an edge

24 REPLIES 24
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Message 1 of 25
Steven.ware
7917 Views, 24 Replies

Can't constrain curved face to an edge

I need to constrain/mate the rounded nose of this plunger to the edge of the threaded hole in an already existing part. We are trying to retro fit a current design with a solution to a problem. I need these parts mated together so I can adjust the size of the plunger to fit into the current design. I have done a lot of searches through the discussion groups as well as online, but to no avail. I did read somewhere that you could use a tangent constraint between a curved face and an edge, but I can’t seem to be able to accomplish this. Anyone have any thoughts on how I could accomplish this?

 

Steven Ware

Autodesk Inventor Professional 2010 SB SP3

XP Pro SP3, 32-Bit, 3.00GB

NVIDIA Quadro FX 370

HP xw4600 Workstation

Steven Ware
Designer
Inventor Pro 2020.2.2 64bit
Windows 10 Pro, 64
24 REPLIES 24
Message 2 of 25
BMiller63
in reply to: Steven.ware

Tangent Constraint

 

edit: sorry I was trying to add the online help for tangent to clarify, but I'm having technical issues doing so.

 

Basically you'll use the buttons on the lower left to flip the solution, I think.

 

Message 3 of 25
Steven.ware
in reply to: BMiller63

I have tried to use the tangent constraint. When I do IV only selects the center point of the hole edge and the center of the radius of the nose. This put the curved face of the nose well into my other part. I need the nose of the plunger to only stay in contact with the hole edge. I have a spring pushing on the plunger to keep them in contact. But until I can keep them touching, I can’t finish updating the rest of the part to fit my design.

 

 

edit: my explanation above was for using the mate constraint. when trying to use a tangent constraint i am unable to select the edge of the hole.

 

Steven Ware

Autodesk Inventor Professional 2010 SB SP3

XP Pro SP3, 32-Bit, 3.00GB

NVIDIA Quadro FX 370

HP xw4600 Workstation

Steven Ware
Designer
Inventor Pro 2020.2.2 64bit
Windows 10 Pro, 64
Message 4 of 25
JDMather
in reply to: Steven.ware

Create sketch arc on center plane of hole the same size as on the plunger part (coincident to projected edge).
Create work point at intersection of axis and arc, same on plunger.

Mate the work points.

 

Attach assembly here if you can't figure it out.


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Message 5 of 25
BMiller63
in reply to: Steven.ware

ahhh, I see. (sorry I didn't think about the edge not being an option to select)

 

try this:

  • constrain the centerlines of the 2 parts
  • then add them both to a contact set and turn on the contact solver
  • carefully slide the pin toward the hole until it contacts and stops
  • then constrain the pin into place using the mate (of flush) and some other faces, but using the predict offset to gather the distance of offset the parts are sitting at.
  • then turn off the contact set options.

 

a video on contact sets:

http://www.youtube.com/watch?v=HSfRBVgPq1g

 

predict offset button

Predict Offset for tangent.png

Message 6 of 25
Steven.ware
in reply to: BMiller63

Thanks for the replies. I have used contact sets recently. That is what I ended up using. I could not get the predict offset to work though. I had the box checked, but it would not recognize the distance. It must not have liked what I was selecting. I have had this situation in the past when I have wanted to constrain a conical face to a hole edge. I ended up using contact sets and offset mates then also. I was hoping someone figured out a better way of constraining different shaped faces to hole edges. It would make life a lot easier.

 

Steven Ware

Autodesk Inventor Professional 2010 SB SP3

XP Pro SP3, 32-Bit, 3.00GB

NVIDIA Quadro FX 370

HP xw4600 Workstation

Steven Ware
Designer
Inventor Pro 2020.2.2 64bit
Windows 10 Pro, 64
Message 7 of 25
JDMather
in reply to: Steven.ware

...you can also Split the the spherical or conical face at the hole diameter to use to Mate or Insert.

 

This is particularly easy to set up if you use multi-body or derived component modeling techniques - change one and the other one changes.


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Message 8 of 25
SBix26
in reply to: JDMather

Another workaround is to add a very small chamfer or fillet to the hole edge, allowing the tanget constraint to be used.  This is more realistic, since there is no such thing as a perfectly sharp hole edge, especially if produced by a top-notch machinist. 

 

That said, I would still like Inventor to be able to constrain a conical or spherical surface to a round edge.  This situation arises fairly frequently in my work.

Message 9 of 25
Steven.ware
in reply to: SBix26

JD

 

I was not able to split the face quite right. I edited the plunger from the assy, did split face, but was unable to select the edge of the hole from my other part as the tool. I could not select any face or edge from my other part. Am I missing something or doing something wrong? Can you explain a little more?

 

Sam,

 

I do understand that there probably would have been a chamfer or radius on the hole due to the machining. When this part was designed it was made from another already released part and modified to add the threaded hole. When the model was created no one added that chamfer. I modified a copy of the model and added the chamfer to the threaded hole, and then I did the tangent constraint. At first it didn’t work, then I flipped the constraint to the inside and it worked just as I needed. This would not have worked on the previous problems that I have recently had, trying to create my original constraint on a conical face to an edge. The work around I has to use is as I started in post 6.

 

Thanks again for the replies.

 

Steven Ware

Autodesk Inventor Professional 2010 SB SP3

XP Pro SP3, 32-Bit, 3.00GB

NVIDIA Quadro FX 370

HP xw4600 Workstation

Steven Ware
Designer
Inventor Pro 2020.2.2 64bit
Windows 10 Pro, 64
Message 10 of 25
jwood14
in reply to: Steven.ware

I am trying to mate these two surfaces.... Any ideas guys? the lighter blue is supposed to ride on the darker blue face, which is tapered... I am a Machinist, I can make this work in the real world, just not in the digital.

Message 11 of 25
jwood14
in reply to: Steven.ware

I am trying to mate these two surfaces.... Any ideas guys? the lighter blue is supposed to ride on the darker blue face, which is tapered... I am a Machinist, I can make this work in the real world, just not in the digital.

Message 12 of 25
JDMather
in reply to: jwood14

Looks to me like it will be a Tangent or maybe a Transitional (with trick).

Can you attach the assembly here?


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Message 13 of 25
jwood14
in reply to: JDMather

Wouldn't I need to attach all the parts?

-Jonathon Wood A-101
Message 14 of 25
JDMather
in reply to: jwood14

Yes, an assembly without part isn't really an assembly.


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Message 15 of 25
jwood14
in reply to: JDMather

I cant add all of the parts since they are for my boss, but I will post what I can.

Message 16 of 25
jwood14
in reply to: jwood14

here are the rest

Message 17 of 25
JDMather
in reply to: jwood14

I do not see any component named "slide" in your assembly.

Did you rename parts?

 

Slide.png

 

 

If I open the file named "slide" this is what I see.

 

slide error.png


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Message 18 of 25
jwood14
in reply to: JDMather

oops, send you another sile, here it is

Message 19 of 25
JDMather
in reply to: jwood14

Ideally what you would have done is Save Copy As the assembly file with a new name with the parts of no relevance removed so that Unresolved errors do not pop up on this end.


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Message 20 of 25
jwood14
in reply to: JDMather

What I did was I restarted from scratch, I went to save it as the same name, I renamed it and forgot to delete the original.

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