Challenge anyone?

[Raider_71]

Hi all,

I have a bit of a challenge I need some help with. So who's up for a challenge?
I need to create a checking fixture component for a tube and need some direction. I know there are some highly skilled IV users out there and I would really appreciate your guidance!

I have created two posts under “customer files” with the zip files needed and which contains all the files and also a doc file explaining what I need to do exactly.

Thanks
Pieter

[JDMather]

Is there a reason you didn't use Derived Components for this? Looks to me like way more work than necessary.

[Anonymous]

How much do we get paid to do your work for you? 🙂

What version??

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
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http://teknigroup.com

[Raider_71]

Hahahaaa... I am using 2008. I would just like to see your approach.... I suppose I have no clue where to start...

[Raider_71]

No reason but how would you construct the surfaces to create the recessed portion? Thats what I am struggling with.

P

[Anonymous]

Create a parting line on each side of the part, then sweep a surface for the
cut.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
260-399-6615
Instructor/Author/Sr. App Engr.
AIP 11SP3, AIP 2008 SP2, PcCillin AV
HP zv5000 AMD64 ( modified)
Geforce Go 440, Driver: .8185, 2GB RAM
XP Pro SP2, Windows Classic Theme
http://teknigroup.com

[JDMather]

Do you really want the recessed portion to be rectangular with 90° corners? Is this a pocket created with an endmill? Tell me a little bit about the function of the part and/or the manufacturing process of the tool. I don't want to spend time on a solution that doesn't really solve the problem.

[Raider_71]

No, it does not have to be 90deg. The start and finish is to locate the part and the recessed area is to check if the part is within spec. Normally 0.25mm. The one I did was just a sample to give you an idea of whats needed.
P

[Raider_71]

Thats exactly what I was thinking but could not get it right. Creating parting lines on a compound angled part does not seem that straight forward.

[JDMather]

>recessed area is to check if the part is within spec. Normally 0.25mm.

So should it offset the actual contours of the part by .25 or is it milled as a simple rectangular pocket?

Are you going to need both sides or only one?

[Raider_71]

Both sides yes and milled as a simple rectangular pocket.

[JDMather]

Hmmm,
Well anyway here was my first effort.
I did a .25 offfset of the part other than the cylindrical ends.

[Raider_71]

Awesome! How did you do that? I would really like to know how you generated the split line/surface to cut the part like that. Did you use Inventor to do this? Please let me know. I am going home now... different timezone, but will have a look tomorrow.
P

[JDMather]

Yes - it was done in Inventor by Sweeping a line along 3D sketch spline

[Raider_71]

Great! Can you send me the part with its history? I would really like to see how you did it. ...begging...begging... 🙂

[Anonymous]

Does your tube need to be so lumpy & bumpy? Looks like a forklift ran over it. In your example the groove has a flat bottom with vertical walls and that's tough to define with that irregular section.

[Raider_71]

At the moment anything will do... even asuming that its an "not so lumpy" pipe. Have you got an idea of how to do it yet?

[Anonymous]

Here's my attempt. I assumed that you don't want the lumps & bumps in the tube so I made one with a constant section. Then I subtracted it from a block and Swept a section with the square corners & the 1mm clearance on the sides. I'm not sure if it's the most efficient method but I think it's reasonably close to what you want.

[Raider_71]

Thanks for the try! I was hoping you would use my part though. Sorry for the misunderstanding here. You see on my part I don't have a "path/centre line" to use for the sweep. This makes it a bit more tricky. JD Mather sent me a file where he got it right but as a base solid part so I could not see how it was done. Now I am back at square one.
The challenge still exists... for me.
Thanks for the try mate.
P

[JDMather]

Start a new ipt file.
Exit sketch mode.
Derived Component and select your original part and Body as Work Surfaces.
Start a 3D sketch.
Sketch a line from centerpoint to centerpoint of cylinder end.
Repeat (in same 3D sketch) for cylinder on other end.
While still in same 3D sketch create a spline from enpoint of first line to centerpoint of each tube circle ending at second line.
Add Smooth constraints at lines and spline.
Create new workplane using beginning point of 3D sketch endpoint of 3D sketch and the point in the arc bend.
Start a new sketch on the workplane and Project Geometry the first line from 3D sketch.
Change the projected geometry to construction.
Create a line near the end of projected geometry.
Add a perpendicular constraint between new line and projected geometry.
Add a coincident constraint between midpoint of new line and the projected geometry.
Sweep as surface (you might also try adding a line at other end and try Loft with centerline instead of Sweep to check the results).