simple, but frustrating..

[tnik]

I'm just trying to extend a set of lines to a plane so they will all be the same height.. I can't get it to work.

I drew the points in 3d (had a list of xyz points to get a contour right) and just can't get the lines to extend.

any help is greatly appreciated

[JerryFlyGuy]

Extending doesn't work w/ 3D sketchs. I'm not sure why you chose a 3D scketch [probably a reason which isn't evident from what you've posted] but I try to avoid them where possible. Unless your doing some Organic shapes they're just a pain in the butttt.

You may be able to grab the end of the line however and then while holding the CRTL button, select the plane you wanted to extend to, this will pop up the constraint's window on the left.. click Coincident and it should [I think] pull the line out to the plane.. then again being a 3D sketch is probably won't.. but its worth a try..

[tnik]

yea, I see that 3d sketches suck. What you suggested didn't work, but thanks anyway.

Reason I chose 3d sketch is we are reverse engineering a part that on the front of it is angled and follows a curve, so we threw the part in our own CMM to pick up various points. (Haas VF-4 with an edge finder.. lol) We picked three points on top of each other (at an angle of course), and several sets around the curve. I couldn't figure out how to use regular sketch to plot 3d points (all the Z levels are different)

if you can't think of anything that might help, I might just have to throw the part back in there and pick up points via the same Z levels and just create a plane for each.

[JerryFlyGuy]

tnik.. If it was me I'd try to do some 3D intersection curves. It sounds like your geometry is a bit complex for going this route however. Well.. not so much the geometry but the CMM data your using.

If you did a profile sketch of your part on the top plane, and then a side view sketch you can do an insert/curves/projected curve. I've included a file showing how it works [ just change the .zip to .sldprt as the forum won't let me attache a .sldprt file] it's a very powerfull tool to get complex 3d curves w/out haveing to resort to that stupid.. #%@#^@%#$@#$@ 3D sketch..
if you get me drift..

I only use the 3D sketch for guide curves in lofted features.. period..

Another option if you have a list of x,y,z points is to do an insert/curves/curves thru xyz you can enter them manually or via a excell file etc.. this will put a 3d curve through all your points however it limit's the control of the curves to some extend..

HTH

[tnik]

Thanks, I'm sure I can use that some how, but not sure how.. I attached a sldprt file, (rename of course) hoping you can help.

on the drawing, I imported a dxf of the profile of the part, and I created 2 curves using the 'create curve with xyz' if you can show me or give some tips on how I can accomplish to create the angle on the profile I'd greatly appreciate it. view from top and you should see what I'm talking about..

the bottom of the drawing is angled out through the radius on both sides, then flows into a 90 degree angle on the left and right edges.

[JerryFlyGuy]

Hrm.. I'm still a bit confused Tnik, looking at the geometry your working with, this all should be fairly easy, however I'm not getting or seeing the end result your trying to accomplish.

Can you take the three views [front top & right] and take screen shots, and then use paint to mark up the pictures and post that?

I'm sure I can help you, I just don't understand at this point, what your trying to do.

Btw, I don't suppose you could post a photo of the part or a portion of it?

It is very possible that what your trying to do is put a sketch on a non-linear surface. This is very easy to do,but I'll need just a little more info to help you w/ it..

[tnik]

here's a couple pictures of the part.. in the dark photo, you can see how it's angled.

edited the dark photo.. looked too dark over on this computer.

and added in a very very very very very crude part file of it.. the blend isn't good but whatcha expect for a 30 second throw together should give some type of idea of what I'm looking for.. just drawing it free hand isn't good enough, I need to use the xyz coordinates that I have.

[JerryFlyGuy]

ahhh.. interesting part I noticed the K1000 riv-nut holes.. I can guess the approximate application

Here's the part as I'd do it. The other way to accomplish this geometry would be to use a sweep with guide curve details or.. a loft and use the loft as a sweep function and have intermediate stations around the bottom side of the curve. This would give you control of the outter edge of the lip, keeping it sqr to the flange [if that is important]

Also its worthy to note that the profile as it stands is a bit rough and could use a little clearning up, the vertical outter edges aren't vertical, and the curved section's don't fair into the outter edges [aren't tanget] if that is a concern, I'm not sure..

anyway you get the idea how to accomplish this regardless..


Hope that helps friend.. ask away if it's not clear or there are other conciderations..

[tnik]

The profile was generated by a true CMM so thats where that came from. what you did helps out greatly and I see I have alot to learn

One question tho, how did you determine the angle of the line for sketch6?

and yea, it is a great part.. I love jobs like this.. supposedly the hole that is in the front right pocket was created by a bullet

[JerryFlyGuy]

One thing you'll learn is that solidworks is a very diverse program. Since I've last posted I thought of another way to do this which is probably the simplest of them all. I'll include it here..

Sketch6 is just a single line sketch on plane3.
All I was trying to do there was to show the program that the transition from sketch4 to sketch 5 was just a straight transition. There was no curves in the actual face of the flange. Each end of that sketch is constrained to the profile sketch [sketch4 & 5] with a pierce constraint. Basically what that is, is where the profile sketch pierces through plane3 [the plane I was sketching on] it attaches the end of the line at that point, if you do it at two points [both ends of the line] then the line is constrained and it indicates what kind of transition the loft is supposed to do. It was used as a 'guide curve' in the loft function. there are three guide curves in that particular loft.

The super simple way of doing this would be to use a surfaced loft, and then thicken it.. here's an example.. The advantage w/ this route is that the surface now has a 'normal' edge. In other words the edge of the flange is sqr to the face of the flange all the way around the curve. This will make it look exactly like the picture.

If your going to use your CMM data to create the inside curve, you'll have to input the data for the entire curve, from start to finish. You can then use the loft tool to loft to that sketch curve. There isn't any way[ that I know of] to use part of a curve and part of a line sketch to 'fill in' the missing geometry. Either it's all there or you do it some other way.

HTH

[JerryFlyGuy]

A couple other things I just thought of.. you could probably also do this w/ the lofted bends feature on the sheet metal tool. One thing that my model's don't do, is take into account the curve in the flange in the Z axis. Doing this part of the model in a sheet metal function would allow you to flatten the flange and then offset the inside edge a certain distance. I'm assuming that the flange is a certain width down the face of the flange, as that would make sense. You would offset the inside edge of the flange by that distance and cut off the excess mat'l, then re-fold the sheet metal part and keep modeling. If you ever tried to do a flat layout of the part, you'd probably generate an error, unless all the additional features came after the suppressed 'flat layout' feature, then they would just suppress and you'd be left w/ the flat layout of the flange only.

Another possible way to do it would be to use dual guide curves and do a lofted cut from the top edge of one side down and around and back up to the other side, the dual guide curves would be created by the x and z cordinates of the side profile only and where they intersect w/ the inside and outside face of the flange.. it's a bit more convoluted but.. when reverse engineering these things, it's just par for the course.

Another thing I've learned when reverse engineering is that often times we spend too much time trying to duplicate a feature that the original designer never gave a second thought to.. As in this case, the width of the flange could very well be just a factor of the blank size that was used. It may not matter at all. Often times parts such as these were installed on an almost 'as built' basis in older a/c, you can't go drill out a bulkhead on one airframe and expect it to fit into a different airframe w/ the exact same rivet holes.. now-a-day's that may not be the case but.. back before about 1970 I'd bet money on 80%+ of the airframes out there, that was how it was done..


I hope all that made sense..

[tnik]

makes sense more and more every day.. thanks for all the help

another question for ya. (going off the attached file)

the DXF file that is imported on Plane7 is the top profile of the part. I'm trying to line the outside curve with all of the angled lines (on the planes in the 'planes' folder) and cant seem to figure it out. I'm sure theres a way to get relations to work, I just can't figure it out.

I did just get the SW2007 bible, so got some reading to do