Wrap command

[Werner.D]

Can anyone help.


I am a fairly new user to ProE but have reasonable experience in Solidworks and Acad. I am trying towrap a compound curve onto a cylinder so I can cut into the cylinder with the wraped curve. This works very easily and straight forward in Solidworks using the Wrap command, however I am unable to achieve the same result using the Wrap command in ProE. I get as far as wrapping the profile but am unable to use it to cut into the cylinder. Can someone please advise me of how to use this command correctly or maybe direct me to the correct command to use. I have exhausted my patience in searching thehelp menu.

 

[jeff4136]

I get the impression you are expecting something like Inventor's Emboss feature (if that means anything to you, I've never used SW). Pro/E doesn't have an equivalent. Once the curve (you wrapping a curve or closed "profile"?) is wrapped use it to create whatever feature you feel will give you the geometry you want.

WF2
2006-01-23_030743_200501071840a_sanity_chk.prt.zip

(FWIW, a sweeping a planar section or emboss won't give you the same geometry.)
Edited by: jeff4136

 

[Werner.D]

Thank you for your help jeff4136. I now have a little more insight than before. Thank you also for the helpful sample model. The only trick I have to work on now is to taper the edges of the cut to point to the centre axis. It is interesting though how easy and straight forward this is in SW and mosttortuous in ProE.

 

[jeff4136]

"... taper ... point to centre ..."

Sounds, again like the Emboss feature. Something like ... 2006-01-24_023534_emboss_like.prt.zip (WF2) ?

If that's not it maybe you can post an example of what you are trying to do (mildly curious what you are making that you'd _Want_ the converging sides).

" ... tortuous ... " If the work you do doesn't routinely demand the additional horsepower Pro/E provides you will probably never come to appreciate the program. I used IV for a few years and regret the money and time wasted.

 

[mgnt8]

I like the variable section sweep in your first model better - this also makes it easier to shape the section with the taper he's looking for. I've never actually modeled with solidworks before so I don't know why thiswould besupposedly so much easier than pro/e. Maybe Werner could enlighten us with some further descriptions or images. IMO the variable section sweep provides some of the most powerfulmodeling functionality & flexibility in the toolbox, particularly if your feature extends through x, y, & z directions. My only frame of reference for comparison would be the Edit > Offset command with Draft Feature, although I don't believe this would work along a 360 degree cylinder. How bout it Werner, how does solidworks accomplish this task so much better?

 

[Werner.D]

As I said earlier, I am a relatively new user and am trying to find my way around ProE. I used solidworks in previous jobs but ProE is the standard for the current company. I am trying to replicate the cutting action of a tool into a cylinder that can move rotationaly as well as along its longitudinal axis as would bepossible in a CNC machining operation. The enclosed SW pictures show a plain cylinder with a circle sketched on a tangental plane. This is then "Wraped" using the wrap command in SW which then direcly "cuts" the wraped profile into the cylinder.(it's possible to "extrude" the same profile). The result is shown and the two cross sections show the difference in draft angle of the profile, minimum at the longitudinal ends and maximum at right angles to the axis. I'm confident that ProE can accomplish the same result but it does not seem to workasstraight forwardas in SW. The actual profile I am trying to create is infortunately classified, however it would be of similar complexity as the one shown in the last picture. (again note the variation in draft angles as the cut propogated to either side of the axis).


2006-01-25_234252_Wrap.zip

 

[jeff4136]

Ok, I think I understand and the emboss_like model should do what you describe. IV's Emboss feature, and I'm assuming the SW equiv, work off surface normal offsets which is why there's max "draft" where there's purely relative axial motion and none where there's purely relative annular motion (the intent of the posted model was to exagerate the effect). If you don't feel like it's right and can post a SW model we can probably make the determination or I might better understand.

That said, I wonder if the geometry in that model and in your pics is really as would be cut using the setup I'm imagining (tube can rotate and translate axially under the cutter and cutter axis intersects tube axis at right angle). If in 3.jpg the extended edges intersect at tube axis then cutter axis would be offset. Does that matter?

I think the easiest way for you to get what you want is to start with a cylindrical surface (not solid), do the wrap and trim the quilt, then thicken.

... (and) If the offset cutter axis isn't what you want it's just a little more complicated; Trim and Thicken using a cutter axis curve then offset "cut" faces to cutter radius and Solidify (I think).
Edited by: jeff4136

 

[mgnt8]

Why not just extrude the section (1st feature) and then add variable draft (2nd feature)? If not then try the Solidify. If you know what the edges will look like on the I.D., then you might try Edit > Project and build a quilt with your two projected boundaries.

 

[jeff4136]

Here ya go.

(WF2) 2006-01-26_140747_prt0001.prt.zip

I'm not sure I thoroughly (it's not a trivial shape) understand all that it says.

From a practical standpoint, I believe I'd discuss it with the machine shop and see what they'd like to see. I have a notion that a cutter axis curve on cylinder is all they'd (want? /) need and a set of surfs that don't really represent the cut would just be a hindrance. If that's true, just model whatever's easy and will serve visualization requirements?

----- or, coming out of tunnel vision mode -----

2006-01-26_155646_prt0001a.prt.zip

This goes back to a variation of the original sanity_check model posted. I think it's probably the quickest and most accurate representation you'll get.
Edited by: jeff4136

 

[Werner.D]

Many thanks jeff4136 and mgnt8.


I think that the last messages have shown what I have beensearching for. It does confirm though that SW is simpler in this instance with the use of one feature command to do the same as 2-3 minimum in ProE. I also agree that the tool offset isa primary design paramater and although the tool is a LASER of 0.14mm dia. I will be taking this into account as the profile requires tolerances of +- 0.01mm . Thematerial thickness is0.5mm and tube diameter 35mm.


Many thanks again.