Yet another AutoCad Inventor Question...

[modular93fox]

Im full of ideas short on expertise with the program that can probally do what I want. Basically I want to make a Y pipe tip for my truck. I made one by hand and came out great. All free hand, but took a while doing it. Well I figured since I have this program, maybe I could do it in pieces, rip each section down the length of the "tube" and make a flat pattern, print it, wrap it around the tube and mark it, cut and weld.. Well I found out real quick.. well 1.5 hrs into it Im not making any progress.

Basicallly, the Y pipe is made out of 2.5" tubing. Say for the long single leg, is .. say 4 inches. then there is 2 small tubes that go from the single to a 45* angle outwards for say... 2 inches and then has a 45* cut to make the extensions parallel to the single. all in all it would be 5 pieces, only the first 3 would need to be in autocad as the 2 legs are strait pipe.
Anyone thats familiar with Inventor and patience with want to lend a hand for the inexperienced... lol

clint

[modular93fox]

hurm, So I have started an IPT file, kinda got one of the middle Y pieces laid out as a 3d Tube... with a wall thickness of .1 (just a number for 3d). Ive managed to get one of the angles somewhat right. Now that I have this part, I am at a loss on how to get this into a flat pattern.. im going to play with it just a few more minutes which will probally turn into another hr... ha.
clint

edit:
found this neat tutorial on the rip tool which i think i need to use once i get the tube in the right shape... problem is when i apply the tutorial to the tube drawing, I cannot apply points to the tube becuase its round... sob

[Bryce]

Hey,

If you want I can spend some time on this next week. I can make you the flat patterns in a DXF file. I use CATIA and I could write down the steps I used. The nomenclature would be different.

I use the sheetmetal design toolbox frequently at work. Its really easy in CATIA.

One quick though tis you may need to trick AutoCAD. You may need to add a split in the tube so it knows where to unfold.

[modular93fox]

I just tried the split in the tube... I think I'm breaking the sheet metal rules... I drew the OD and ID tube in the regular program, extruded it so it looks like a piece of exhaus tube and then converted to sheetmetal. I think because I did not create any bends, it doesnt know what to unfold.

clint

[Bryce]

In CATIA i use "undeveloped" for curved surfaces, I just remembered that right now.

[modular93fox]

Heres a screen shot of the idea... I need to look through the software I have and I think I have catia 5 - 19... never used it but maybe I will load it up and give it a try too. The exhuast piping I will be using is 2.5" and the 2 tips have a .5 spacing in the middle so I can get my welder in between the 2.
Thanks Bryce for your help.
Clint

[Bryce]

If i was using CATIA I would use boolean operations. I would build two tubes and use "add" under boolean.

Or you could use sweep and stop short then create a pad from the tube and make the length "up to next"

[Bryce]

Post up a top down view with dimensions of your sweep lines and I will play with it on monday.

[modular93fox]

After redrawing the 2nd tube, the sweep tool worked. So now that the 2 tubes are hole, I deleted the faces that were inside the tube. So now I have the finished product in 3d, but thats it.. Im going to play around and see if i can seperate each piece.

[69stang]

I don't have a lot of experience with Inventor but something to think about, in solidworks it needs a section of flat geometry, a reference to bend from. In this situation I include a small flat strip in my geometry, as minimal as possible, to work around the issue.

[modular93fox]

I started to try that but I could not figure out that one either. I happened to hit f1 by accident while hovering over the contour roll.... that gave the sheet metal rules to the tube that it created. So what I did was like it said... create one line of design... i made it 5 inches, and the axis, 1.25" away (with dimeinson and constrained it). it said it applied the unfold rules to it, but when i hit Unfold, theres no "stationary reference"... do i need to make something else or add a plain?

edit:After trying something dumb I can get the required reference... instetad of 360"... i can put in 359* and it willl display the reference and it will unfold. So now I will try and make some cuts and see if it transferes over....
clint

another edit: found it transferes, after watching another tutorial on tring to find unfolding tutorials, i found this one thats unrelated but it walks through putting an angle on a work plane. The angle on the work plane will let me draw the intersecting pipe.... This might allow me to do what I want.... Im play around with this some more.. ha... this was supposed to be easy and faster than me eye balling it.. haha

[modular93fox]

Finally got a flat pattern for the 1st part of the "tip"... the one that could have been cut with a chop saw :) The way I did it was pretty much turn the sheet metal features and functions into a "tubing notcher" like machine.... creating a work plane at a given angle, create a 2.5" circle on the angled plane, extrude cut - all... the cut features transfers to the flat pattern - and thats what i was looking for... now the harder one, the tube part thats in the middle where the 2 pipes turn into 1... once I get it, Ill post it up :)
thanks for your help Bryce and 69stang,
clint

[modular93fox]

Im stuck again...
edit.. winged it again... haha

[modular93fox]

my my my I hate inventor... mostly because Im lacking the know how. So ive managed to create a Tube structure that I can unfold. Ive also managed to get the complicated 3 cut tube laid out correctly via the CUT tool, and then inventor gives me this non sense :
Part1: Errors occurred during update
Part1 (Flat Pattern): Errors occurred during update
Definition1: Could not build this ASMFlatPattern
Modeling failure in ASM. Redefine inputs.

If I take out the top cut, leaving only 2, it will make still give error... if I remove the 2nd cut at the bottom, the bottom has 2 angles, it will be ok and no message. .. any insite? Maybe I will load up catia and play in it for a while... ?
clint

just like the equipment at work... theres a work around for my situation... if I leave a sliver of "material", It will create the flat pattern.... no big deal as when I trace it to the tube, I will just make the line extend with the cut off wheel...and since the sliver is about .1 inch.. no biggie... its just wierd..
clint

[modular93fox]

whoo hoo. exported the flat pattern to dwg format, printed to the inject printer, cut out with a razor and traced it to the pipe... it took only a few minutes to cut out each piece and its surprizingly spot on!... ran out of daylight so I didnt weld it up.. mearly taped it together.. I spent a few hours changing and doing exhuast work on my friends dads 2011 SS.
thanks fellas,
clint

[Bryce]

Awesome, good job! Way to figure it out.

[Rhino]

found this neat tutorial on the rip tool which i think i need to use once i get the tube in the right shape... problem is when i apply the tutorial to the tube drawing, I cannot apply points to the tube becuase its round... sob

I ran into this issue last night. To use the rip tool you need to create a new 2d sketch on the surface you want to split, project geometry from the underlying object, then place the points on the edges of the object, along that projected geometry. This creates a break in the surface, similar to what is happening by adding the flat geometry to the loop.

So far I haven't had much luck in getting a flat pattern out of anything I've converted to sheetmetal. Starting with a new sheetmetal part works much more reliably for me.

EDIT: Also, I don't believe you're leaving a metal ribbon in that component. I think it's either an unconsumed sketch, or you've set the visibility in the sketch consumed by the extrusion.