LOFTing goes ALOFT

[Anonymous]

What's the trick to lofting along a curved path?

I've tried just about everything I can think of and just can't get a
decent loft to follow a path (radial/curved) unless there's 3 sections
and the loft and you only loft across one arc (each arch needing
seperate lofts).

The profile is the same except it get's "taller" as it follows a radial
with. Imagine an "S" shape, where the top edge slopes down as you
follow to the middle and back up (different height than the beginning)
toward the end of the "S".

I've even go a 3d sketch along the path I need and it still won't accept
it as a rail ("Unsuccessful operation").

What's the trick?

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

What version of Inventor are you using?

In Inventor 7 it's a pain because you need to create a rail at every point
in the crossection where two entities touch. If you're lofting a rectangle
you will need four rails, one for each corner. I triangle will need three,
and so on.

In IV8 they've added the ability to just place 1 rail and it should
following it, but I haven't tried it out yet.

"Darren J. Young" wrote in message
news:MPG.1a39242bbefdb46a989687@discussion.autodesk.com...
> What's the trick to lofting along a curved path?
>
> I've tried just about everything I can think of and just can't get a
> decent loft to follow a path (radial/curved) unless there's 3 sections
> and the loft and you only loft across one arc (each arch needing
> seperate lofts).
>
> The profile is the same except it get's "taller" as it follows a radial
> with. Imagine an "S" shape, where the top edge slopes down as you
> follow to the middle and back up (different height than the beginning)
> toward the end of the "S".
>
> I've even go a 3d sketch along the path I need and it still won't accept
> it as a rail ("Unsuccessful operation").
>
> What's the trick?
>
> --
> Darren J. Young
> CAD/CAM Systems Developer
>
> Cold Spring Granite Company
> 202 South Third Avenue
> Cold Spring, Minnesota 56320
>
> Email: dyoung@coldspringgranite.com
> Phone: (320) 685-5045
> Fax: (320) 685-5052

[Anonymous]

> What version of Inventor are you using?

Which version? Take you pick. 😉 Tried it in 6 & 8. I suppose I could
load up 7 and try it there but I doubt it would do any good.

Initially, I took some geometry (just one ramped arc segment) created by
another user that they couldn't get to work in 6. Bring it into 8, I
removed all dimensions, work points, etc added a couple constraints and
it worked with 2 sections (start and end) and selecting an arc to
follow. Unfortunately starting from scratch, I couldn't get it to work
again.

I've went as far as having a 3d sketch with the 3 ramped arc segments I
need and it wouldn't even follow that.

The only way I could do it is to have the 2 end arcs, each have 3
sections (start, middle and end) which is a 3pt arc so loft creates what
I need without any rails. I'd then project the ends of each loft and
used a center sketch for the middle arc (that connects the other two) to
make a 3rd loft.

Just seems as though you could give it all your sections, pick a sketch
with the 2d path it should follow, and have it created properly.

Ideally, I'd like to take a 2d profile and sweep(preferably loft) it
along a 3d path and have it generated that any section would have the
same sketch profile normal (perpendicular) to the 3d arced path.

> In Inventor 7 it's a pain because you need to create a rail at every point
> in the crossection where two entities touch. If you're lofting a rectangle
> you will need four rails, one for each corner. I triangle will need three,
> and so on.

That's convenient, especially for profiles with lots of tangent radial
arcs. Sheesh!

> In IV8 they've added the ability to just place 1 rail and it should
> following it, but I haven't tried it out yet.

I did get it to work once in 8 but haven't since. I suppose something
isn't just right with my constraints. I've got 4 sections all the ends
of each of 3 arcs. (The center arc mates with the other two). Tried
selecting the arcs on the plan view sketch for it to follow (they should
all intersect the profiles and be constrained) but it still lofts
straight from section to section.

If anyone wants to look at what I'm trying to do, just reply and I can
post the files to the appropriate newsgroup. I'm not going to upload
them unless someone wants to look at them. I've wasted enough time
myself with this, I'm not going to *ask* anyone else to do the same.

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

Try this site:

http://usa.autodesk.com/adsk/servlet/index?siteID=123112&id=3017577

and this video:

End-to-End Autodesk Inventor Unified Shape Description Demonstration

This is pretty good concerning lofts

[Anonymous]

I'm not sure if this helps, but one trick for loft is that you sometimes
need a "second click".

After you select a 2D or 3D sketch ("first click") for a section or rail,
the selected sketch might contain multiple loops for the section or multiple
rail curves. In that case, you need to select a specific loop or rail curve
you want ("second click").

Glenn

"Darren J. Young" wrote in message
news:MPG.1a39242bbefdb46a989687@discussion.autodesk.com...
> What's the trick to lofting along a curved path?

[Anonymous]

If it's not too much trouble, please poet your file, I'ld like to look at
it.

Joe Bartels

[Anonymous]

Try going to the transitions tab and unchecking Automatic Mapping.
"Darren J. Young" wrote in message
news:MPG.1a39242bbefdb46a989687@discussion.autodesk.com...
> What's the trick to lofting along a curved path?
>
> I've tried just about everything I can think of and just can't get a
> decent loft to follow a path (radial/curved) unless there's 3 sections
> and the loft and you only loft across one arc (each arch needing
> seperate lofts).
>
> The profile is the same except it get's "taller" as it follows a radial
> with. Imagine an "S" shape, where the top edge slopes down as you
> follow to the middle and back up (different height than the beginning)
> toward the end of the "S".
>
> I've even go a 3d sketch along the path I need and it still won't accept
> it as a rail ("Unsuccessful operation").
>
> What's the trick?
>
> --
> Darren J. Young
> CAD/CAM Systems Developer
>
> Cold Spring Granite Company
> 202 South Third Avenue
> Cold Spring, Minnesota 56320
>
> Email: dyoung@coldspringgranite.com
> Phone: (320) 685-5045
> Fax: (320) 685-5052

[xavierl]

I found that practicing lofting with circular loops can be very frustrating. Sometimes the rails you put in dont connect properly (in iv7) .Try starting out with loops made up of straight lines. There is something funny about the way inventor defines a circle. It does not seem to have the convenient quadrants that it had in autocad, that you could snap to.

regards, Frans X Liebenberg (still waiting for iv8)

[Anonymous]

I just looked at the loft and the only problem was that you had too much
geometry on your rail sketch. To get around this I created a new sketch and
projected up only the geometry for the rail. I posted my file on the CF for
you to look at. I was then able to pick all of the loft sections and the
one rail and finish it in one loft feature.

I'ld enjoy seeing some of the stuff you do at one of the Minnesota Inventor
user group meetings.

Joe Bartels

[Anonymous]

In article , hoser_71@yahoo.com says...
> If it's not too much trouble, please poet your file, I'ld like to look at
> it.

Threw it in Inventor.Customerfiles.

If you look at the section profiles I have, You'll see they are in two
parts. A rectangle and an upper part. The rectangle was used only as a
means to help get the proper heights based on the drawings we received.

Unlimately, all we need is the top ~9" of the thing.

I'd like to be able to loft it all in one loft following the plan view
arcs.

Ultimately, I'd like the profile to actually be lofted so that's it's
always perpendicular to the path it's lofted along. As it is not, as the
profiles lofts along (gently up and down) it's slightly at an angle.
Almost a combination of a sweep & loft.

The issue I have is more of the loft tutorials and examples, show the
path (rail) construction in Inventor being done free form or from other
existing geomtry. Most always here, there's no other geometry to
generate the loft rails and that path comes in from an AutoCAD drawing
or whatever else we receive.

Any comments (good or bad) welcome.


--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

> I'm not sure if this helps, but one trick for loft is that you sometimes
> need a "second click".
>
> After you select a 2D or 3D sketch ("first click") for a section or rail,
> the selected sketch might contain multiple loops for the section or multiple
> rail curves. In that case, you need to select a specific loop or rail curve
> you want ("second click").

Thanks for the suggestion but I've tried that. Still doesn't do the
trick.

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

> Try this site:

http://usa.autodesk.com/adsk/servlet/index?siteID=123112&id=3017577

and this video:

End-to-End Autodesk Inventor Unified Shape Description Demonstration

This is pretty good concerning lofts

Thanks for the tutorial. Does it appear ok to you? It look horrible to
me. I'm running 1600x1200 resolution with 32bit color. Tried lower
resolution settings (32 bit color is as high as It'll go) and the text
is still unreadable. Perhaps we'll have to add a few more hamster cage
wheels to speed up out Internet connection. 😉

I was able to get the just of what they were doing. However, every
tutorial I've seen shows a spline being drawn (usually freehand) in
Inventor. We typically have defined geometry (most often coming from
AutoCAD) which doesn't lend well the loft rails.

The worse part is, any of the people here can do it in MDT in less than
1/2 the time as it takes in Inventor. IMO, that should be just the
opposite so I'm looking for a process to speed up what we are doing.


--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

The problem with your rail sketch is that it has too much geometry. The
sketch should only have the rail geometry, with no construction geometry. I
would create a new sktech over the rail sketch, and then just project up the
rail geometry. After that it's easy to make the loft in one feature. I
posted the part on the cf.

[xavierl]

darren, did you know, lofting the mid section you do not have to make 3 sketches. you can loft off the end face of a solid. so you would only have needed 1 sketch in the middle and the 2 solids.

Each rail has to be a separate sketch. ie 4 rails = 4 sketches.

You can only bring in 2d flat dwgs onto a sketch plane. So importing a 3d spline as a rail, is still a wish list item.

The other tedious item is that you can only use a rail once. If you wanted to loft a bit further along ,you have to redo the rail.

The other wish list item for me is the ability to import a 3d wireframe from autocad to inventor.(this can be done in SW or C...a).

frans x liebenberg.

[Anonymous]

> I found that practicing lofting with circular loops can be very frustrating. Sometimes the rails you put in dont connect properly (in iv7) .Try starting out with loops made up of straight lines. There is something funny about the way inventor defines a circle. It does not seem to have the convenient quadrants that it had in autocad, that you could snap to.

> regards, Frans X Liebenberg (still waiting for iv8)

I tried that Frans. If you look at the file I uploaded, and view one of
the sketches, you'll see that there's a "rectangular" component to the
sketch. That's all that was there when I was playing with the lofting.
Just lofting rectangles of varying heights (same width) along a series
or 3 arcs.

The top profile wasn't added until later (when I gave up "playing" and
had to get our user a working files) then I just redefined the loft
sections.

Even with just the rectangles, I couldn't get it to loft properly across
all arcs. I had to use 3 profiles on each arc and loft each arc with no
rails to get what I wanted. The 3rd profiles for each arc made Inventor
hold to the line of the arc so it worked in this case, but if I had a
splined path, I think I'd need a few hundred more section profiles.

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

In article <859F087A70A3AE483115809486BA2612@in.WebX.maYIadrTaRb>,
hoser_71@yahoo.com says...
> I just looked at the loft and the only problem was that you had too much
> geometry on your rail sketch. To get around this I created a new sketch and
> projected up only the geometry for the rail. I posted my file on the CF for
> you to look at. I was then able to pick all of the loft sections and the
> one rail and finish it in one loft feature.

Hey! They you go. I knew there was a "trick". Being that when selecting
the profiles, of there's multiple loops you need to pick twice
sometimes, it also appeared to me that when selecting the rail, a double
pick was one order, once to select the "sketch" and the other time to
select the profile in the sketch.

I tried what you suggested in In and omitted the center profiles, using
only those at the beginning and end of each arc and it worked like a
charm.

I also tried the same thing in 6 (the production version here) and as
someone pointed out yesterday, a rail at each place where your lofted
profiles has an entity touching another is in order.

> I'ld enjoy seeing some of the stuff you do at one of the Minnesota Inventor
> user group meetings.

Being that's it's granite, I don't know that I could lug in any pieces.
Might be a bit heavy. 😉

We do a lot of stuff here. Cemetery memorials, mausoleums, granite for
industrial applications, structural cladding/building facing, paving,
etc.

The profile you saw going to end up being wall cap for a wall at the
Visitors Center of the US Capital. If you ever get to Nashville, in
front
of their state capital is a state bicentennial plaza with a lot of
granite provided by us. Part of that is a 200 foot map of Tennessee
(complete with city/county names, lakes, rivers, etc.) all paved out of
granite. FDR Memorial in Washington DC was done by us as well.

Most of the work here doesn't involve 3d. Inventor so far hasn't been
used (mainly MDT) for the 3d work and I'm working on getting people
switched over to Inventor. Things like curved staircase, etc where the
piece ends up ramping and twisting is a prime candidate for 3d.

Didn't realize you were local to the area. You'll have to introduce
yourself at the next user group meeting. I haven't hit them regularly in
a while but I do go. Perhaps you've noticed the long haired redhead.
That would
be me.

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

> darren, did you know, lofting the mid section you do not have to make 3 sketches. you can loft off the end face of a solid. so you would only have needed 1 sketch in the middle and the 2 solids.


No I didn't realize that Frans. Thanks for pointing it out. Considering
the time I spent bumping my head into the wall until Joe Bartels ponited
me in the right direction, I didn't even try anything that would seem to
me to be a "shortcut".

The only reason the mid sketch was done on any of the arcs was because I
lofted each arc separately and needed 3 profiles to get it to loft
properly before I knew about having only the rail and no other geometry
on the rail sketch.

In other cases, I may need extra profiles if the height varied up and
down more along each arc.

> Each rail has to be a separate sketch. ie 4 rails = 4 sketches.


Be nice if they threw little tidbits like that in the help system. 😉

> You can only bring in 2d flat dwgs onto a sketch plane. So importing a 3d spline as a rail, is still a wish list item.

> The other tedious item is that you can only use a rail once. If you wanted to loft a bit further along ,you have to redo the rail.

> The other wish list item for me is the ability to import a 3d wireframe from autocad to inventor.(this can be done in SW or C...a).


What about a 3d sketch? Just for the heck of it, I made 2 copies of a
"rectangular" wall. In one copy, I deleted all the faces except the top,
leaving just a surface. The other, I did the same thing only left the
front face. I then generated new geometry on a 3d sketch where the 2
surfaces intersected. I wasn't able to loft along that.

Of course, all I'm really concerned with is the top of the sample I
provided which really should be swept so the profile stays perpendicular
to the rise and fall and curves of the 3d sketch.

The lofting I did was more for trying to get the elevations into
Inventor. The cap is that wall is the only thing being produced. Any
pointers on getting that swept/lofted across so that the profile is
always perpendicular to the 3d path?

--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052

[Anonymous]

I'm glad it worked out, I had a feeling there was an easier way to get it
done.

Maybe the next time you make it for the user group meeting yuo can bring in
a 3D model. I think I'm going to bring in a big assembly of some of the
stuff we do. I recently moved back to MN from Chicago so I've only been
able to make the past couple of meetings. It's good to see some other MN
people on this group though.

You might want to get Larry Goodwin from Autodesk in to help getting your
other guys to switch.


--
Joe Bartels
Schwing America

P4 2.4 GHz
Win 2000 SP3
1 Gb RAM
NVIDIA Quadro4 750 XGL
6.14.01.4403

[Anonymous]

> I'm glad it worked out, I had a feeling there was an easier way to get it
> done.

Some of it is just me being new here and coming into a project in mid
stream trying to understand where everybody got the data that they have.
I'm starting to get a feel for what we are given and how we should
approach it in Inventor. The few times anybody has done anything, it
typically starts in AutoCAD, moves to Inventor then back to AutoCAD.
Some of these jobs like this I think the need to do start to finish in
Inventor but nobody has had the time to get it properly setup until the
hired me.

> Maybe the next time you make it for the user group meeting yuo can bring in
> a 3D model. I think I'm going to bring in a big assembly of some of the
> stuff we do. I recently moved back to MN from Chicago so I've only been
> able to make the past couple of meetings. It's good to see some other MN
> people on this group though.

I don't think I've made the last couple so I likely didn't run into you
then. I'll see if I can scrape together a few examples although Inventor
models will be scarce. MDT or plain AutoCAD is more likely.

I've still got a long ways to go to develop a good process for this type
of ramp & twist work. After it's modeled, it get's broken into smaller
pieces so I'd like to automate that process so everyone here doesn't
need to know how to use trig in their parameters to break everything
into certain length pieces.

> You might want to get Larry Goodwin from Autodesk in to help getting your
> other guys to switch.

Yup. I know Larry. He works with a couple of my clients (from my
personal business) and he's hoping to get out here sometime when he's in
MN next and has a free moment. I ran into him in Chicago on Nov 5th
while I was attending Autodesk Developer Days and we were planning on
meeting for dinner on the 6th to talk inventor over a little chow but at
the last minute he got rerouted back to Michigan (my home state).


--
Darren J. Young
CAD/CAM Systems Developer

Cold Spring Granite Company
202 South Third Avenue
Cold Spring, Minnesota 56320

Email: dyoung@coldspringgranite.com
Phone: (320) 685-5045
Fax: (320) 685-5052