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Frame generator notching/unfolding issues

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Message 1 of 23
sailah
2937 Views, 22 Replies

Frame generator notching/unfolding issues

Hi,

 

Please forgive my rookie status here, just learning Inventor 2014.  I have gotten the basics and am looking to draw up a mtorcycle frame based on dimensions I have in the shop.  I'm just playing around at this point and sketched a trellis frame and used 3/4" ANSI pipe for the tubes.  In reality I will be using 1" DOM 0.065" wall tubing.

 

  I notched a couple of the tubes and can isolate/open those individual parts.  I have (tried to) follow a couple tutorials on how to "unfold" or rip the notched tube so that I can print out a template, wrap it around the tube and cut/cope it in the shop.

 

I keep getting an error message saying it can't rip it.  Now I drew a tube myself in another part file just by extruding a couple circles and it ripped that just fine, and would unfold it.

 

Is it the ANSI profile I am using from CC?  Is it because it is notched?

 

To be honest I couldn't follow the steps in the following http://forums.autodesk.com/t5/Inventor-General/Unfold-a-tube/td-p/3168764

 

I tried to thicken the part, fail haha.  I'm not sure what I should be doing here.  I can thicken it fine, but then I can't "delete face solid lump"

 

Again, sorry about the beginner question I'm really starting from the bottom here

 

 

22 REPLIES 22
Message 2 of 23
BarryZA
in reply to: sailah

Unfold is only available in the sheet metal environment and does not overlap into FG. New Part - sketch your profile- convert to sheet metal, set your thickness, proceed and then add your rip.
Message 3 of 23
JDMather
in reply to: sailah

Try this one.

 


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Message 4 of 23
sailah
in reply to: JDMather

JD,

 

Yes thanks I downloaded the part and was able to unwrap it easily.  So I guess the question is how do I get from my part to the one you created?  I will be creating probably 25 of these parts so understanding how to do it is important to me.

 

What I can do:

 

  • I can open each part in standard.
  • I can click the "convert to sheetmetal".  I do get a message telling me to ensure that the part is of uniform thickness.  So I have been going into sheet metal thickness and manually setting the thickness to 0.065".  Not sure if this is correct method

 

I seem to have the most trouble with the "thickening" of the part and that stalls everything else out.

 

  • why am I doing that?
  • which direction do I thicken?  The OD of the tube is the most critical.
  • Can I somehow get a steel structure in steel tubing?  I looked and anything in ANSI seems to be pipe only.  Ideally I would like to author a steel tube myself, but when I get to the author dialogue box with an extruded tube I made it doesn't play nice with me. Of course if I am missing a stock tube in CC, that would be much easier.

Once I get the part "thickened", which i can do, it just makes the whole part thicker and I can't seem to delete lump anything.

 

I know these are basic questions and I appreciate the time to help me, thanks

 

This is basically what I am shooting to create

 

 

 

Peter

Message 5 of 23
sailah
in reply to: BarryZA

Barry,

 

Thanks I'm slowly working my way into this.  I am trying to create a tube chassis that I will build from 0.75, 1 & 1.25" OD tubing.  Fortunately I'm better at fabricating metal than using computers.  I attached a file to teh above post to show essentially what I want to do.

 

I was under the impression that frame generator was the best method to do this, but I defer to anyones expertise here.  I am slowly learning to draw lines in 2 planes and then intersect them to create a 3d line.  I can then sweep those lines to do the same thing, but if I ever have t go back and change things, it seems that would be very cumbersome to change.

 

I have the engine and most of the important bits jigged up on a table, the engine I plan to have 3d scanned.   Building and sketching a wireframe that included the important pickup points would be great.  The I could simply point and click where I wanted 3/4" tubing and others where I want 1".  But to be able to quickly modify a "base" wireframe would be very helpful.  

 

All this Inventor stuff is so new, I come form learning Rhino about 10 years ago and it is an eye opener for sure how powerful these new programs are.

 

Thanks again for the helpful posts.

 

Peter

Message 6 of 23
blair
in reply to: sailah

One of the problems with Sheet-Metal, is when you cut the material at an angle to the surface. This will cause Inventor to throw up the thickness error. All cuts under the current releases of Inventor must have the sheet-metal cut 90 deg to the surface. You can't have a cut that tapers out to a point or sharp edge.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Delta Tau Chi ΔΤΧ

Message 7 of 23
sailah
in reply to: blair

Blair, so if I understand, the sharp edge of my part is what is creating the error, thus the need to thicken the part and create a part with no draft?  If that is correct makes sense.  So now I need to figure out how to create that thickened part and unfold it...

 

Thanks

 

Peter

Message 8 of 23
JDMather
in reply to: sailah


@sailah wrote:
 

What I can do:

 been going into sheet metal thickness and manually setting the thickness to 0.065".  

 ...

 


The part you attached does not have a wall thickness of 0.065" ( I measured 0.113" - that is what you need to set as your sheet metal style thickness).

You do not need to use Thicken feature technique, your template does not need to be precise at the cut edge (perpendicular to face).

 

Once you figure out the process you will then need to learn to edit the Frame Generator library to add the tube profile of your actual tube (I am assuming it is not already there, since you didn't use it for this example).

 

Hollar back if you still can't figure out what I did.


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Message 9 of 23
blair
in reply to: sailah

Yes, as long as the edge is perpendicular to the face you are fine.

Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Message 10 of 23
sailah
in reply to: sailah

Jd, sorry you are correct I used 0.113" as that part I posted was using ansi pipe. I did figure out how to post a new steel tube to content center.

I'll horse around with the part you did and see if I can figure out the procedure. The parts in the future will have both ends notched if that matters.

Thanks as usual
Message 11 of 23
sailah
in reply to: sailah

JD, 

 

I traced your steps in the part you sent and tried it on my own.  I saw you put a circle on the ID of the tube, a construction line from center point to outside of circle, and another construction circle as the OD.  I got the part to rip and unfold, so thanks!!

 

Then I decided I would get fancy and tried it on a part with both ends notched.  Fail.  Is it possible?

Message 12 of 23
JDMather
in reply to: sailah

I did not see any attempt in your file.

See attached for one "solution".

 

If you need a very precise template then the Thicken of a surface body will be required.


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Message 13 of 23
sailah
in reply to: JDMather

JD

 

I tried to trace back through what you did but it's way over my head at this point.  I think it'll be faster to use an endmill and grinder and make the part fit on the jig than to try and make templates for every tube.

 

I appreciate all your efforts, maybe I can revisit it in time after I get more experience.

 

Thanks

 

Peter

Message 14 of 23
BarryZA
in reply to: sailah

I know EXACTLY how you feel.

 

But, once you get it right you can use it forever, and prototyping etc. in Inventor is 1000% faster. It will give you an output that will put you in a different league.

 

I've spent many days and nights figuring out workflows for projects, starting over and over and it is worth it. Smiley Happy

Message 15 of 23
JDMather
in reply to: sailah

If you are still around I can explain what I did (it was really quite simple once you know the trick).


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Message 16 of 23
sailah
in reply to: BarryZA

Barry,

 

Totally agree, it's been a steep learning curve, and I think I need to get some more practice time in before I start trying techniques.  Problem is this isn't even close to work related so my spare time to devote to learning a complex program is limited.  I can draw small brackets and such easily, and mostly export the face right to the waterjet machine to cut parts.  That I have gotten very good at.  But a large tube chassis is for sure my most ambitious project to date.

 

I'm just very clumsy and slow and it takes forever to learn what you all do so quickly.  Analogies abound about practice making perfect.  Just finding the time to devote.

 

I'm sure I'll have more questions as time goes on.  And I do plan to keep at this tube ripping thing.  I just spent hours trying last night and kept failing.  I'm not the most patient person in the world too haha.  Then JD swoops in with fix after fix, I finally had to back away as my computer almost got ventilated lol.

 

Peter

Message 17 of 23
sailah
in reply to: JDMather

JD 

 

I'm still here and very willing to learn.  I saw you had created a lot of work planes in that part, I'm slowly learning how/why I need work planes especially on parts that don't have planar surfaces.  But I'm still very clumsy and slow at it and struggle to pick the right work plane to use.

 

Thanks for your repeated patience with me.

 

Peter

Message 18 of 23
JDMather
in reply to: sailah

I did not create any workplanes.

Those were created by the Frame Generator when you were trimming/mitering or whatever.

 

I tried to do a Rip feature, but could not get that to work.

So I manually did the same thing that rip does.

 

When you roll up a flat to cylinder the faces form a pie shape.

In the file I attached earlier I made the angle for the pie wedge very small.


In this attached file I increased the angle for the pie wedge and left the sketch (I named Rip Sketch) visible so that you can clearly see what I did.

 

Project Geometry the edge of the pipe.

Create horizontal construction line.

Create angled line.

Mirror the angled line to the other side.

Dimension the angle (make very small for reduced Gap Size).

Split the part with the wedge.


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Message 19 of 23
sailah
in reply to: JDMather

JD,

 

I'm getting there... I followed your model and built the pie wedge.  And successfully unrolled it.  So then I decided to try again and drew up a quick wireframe and built it out using frame generator, same ANSI 3/4" pipe I did the others from.  Notched it.  Then I open the individual part.  Good so far.  Drew my pie shape.  There were these "tags" lef over from the notch so I used delete faces and removed them.

 

Then I ran into an error message preventing me from going to sheet metal.  See attached screen shot.

 

I'm doing my best to not go to the shop and get a BFH...

 

 

Message 20 of 23
graemev
in reply to: sailah

Watch out with the Unfold tool if you're intending to make paper wrap-arounds for marking the tubing.  As I understand them, the sheetmetal tools unfold using the K-factor as determined by the material setup and will likely generate a pattern profile geometrically appropriate for somewhere in the middle of the material, not at its outer surface.

 

I have template generating files for doing exactly what you intend.  (Both end cut and trunk port.)  We use them here for piping spools - laterals, wyes, and tees, reducing or otherwise - and plot them on roller-bed plotters for the boys in the shop to transfer onto the pipe trunks and branches.  The files are parameter driven, including wall thickness, to yield the outer surface profile of the intersection and the projected inner surface intersection.  They are also marked with centerlines to denote where the branch centerline meets the trunk outer surface and also the centerline-centerline location usually dimensioned on piping isometric layouts.  This allows some judgement on behalf of the fitter to determine where and how to manage weld bevels and avoid the wafer thin pointy bits of size-on-size intersections.  The trunk port template generates the intersection of the interior of the branch meeting the exterior of the trunk, as would be cut for stub-on type fit up.

 

PM me if you'd like a copy.

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