Helix from a point
Ilker Uludag
playing the angle,However If I have a point why can't I select that point as
a start location?
Ilker Uludag
Edward T Eaton
in an enhancement request if you want to simplify this process. While you
are at it, you might want to add some other enhancement requests that are
indicated by the various awkward steps in achieving your task (listed at the
end of this post)
The workaround in SW2001 is:
draw the circle that will be the base of your helix.
in the same sketch, draw a horizontal centerline coincident to the
centerpoint of the circle.
in the same sketch, draw a line coincident with the centerpoint of the
circle and the point on that circle that you want the helix to start from.
Add an angular dimension between the two centerlines. If you can, have the
angular dimension drive the location of the point that you want the helix to
start from. However, if your design intent requires that the point drive
the location of the line (your starting point is dictated by something else
in the tree), let that angular dimension be a driven dimension.
Close out of the sketch.
Highlight the sketch, and use it to make a helix.
After the helix is made, go to tools>equations. The equation dialog box
will pop up.
Hit the 'Add' button
When the new equation dialog box pops up, move your cursor to the feature
tree and double click the helix feature.
Single click the blue angular dimension that will pop up on the screen -
this will add this dimension to the equation.
Once that dimension name appears in the 'new equation dialog box', add the
equal sign (=).
Now hit the plus sign next to the helix feature so you can see the sketch
(*). Double click the icon for the sketch so its angular dimension pops up.
Single click the angular dimension to add it to the equation. (note: If
that angular dimension is driven, SolidWorks will give you a warning
dialog; just hit 'yes' when it pops up- there is nothing wrong with using a
driven dimension to the right of an equal sign in an equation).
Now that the equation is done, hit OK. Hit OK again to close out of the
equation dialog box.
When you rebuild, your helix will start at the point. (**)
----------------------------------------------
You may ask yourself - why don't I just link the values between the two
angles, instead of writing an equation? This is because SolidWorks will
give you an error when you try to link them, stating that 'An incompatible
range of values make these dimensions unlinkable'. (SW2001 - SP2) Is this
a bug or not? If it is not, it is certainly sloppy interface design (unless
someone can tell me a good reason that two angular dimensions have
incompatible ranges of values). I am already unhappy about the prospects
of reporting this, but I will get around to it on Tuesday or Wednesday.
You may also ask yourself, why is everything above written for SW2001? This
is because you can't access the angular dimension in a helix in SW200, or at
least not in SP10. Good job to the programmers for allowing the start angle
of a helix to pop up.
They have got to ramp up their focus on making things like this consistent
across the entire program or SW will be more, not less, difficult to use!
Good job on this one improvement - give me a call if you want dozens more.
-------------------------------------------------------
notes:
(*) if you work with the property manager enabled, you will not be able to
do this right away. The property manager will make it impossible to double
click the sketch to get its dimensions on the screen - double clicking the
sketch icon wont even work on the flyout feature manager. So, in order to
complete this step, you will either have to a) work with the property
manager disabled, b) work with a split feature tree, or c)toggle from the
property manager to the feature manager.
(**) this assumes that the sketch used to define the helix doesn't have an
unusual 'horizontal' . If you have rotated the sketch using
'sketch-modify', or if the sketch is drawn on a goofy plane or face, the
helix might start anywhere. You will have to correct for the rotation of
the sketch Horizontal in order for this to work reliably, either by using
sketch-modify or adding some extra terms to the equation to correct for the
odd rotation.
--------------------------------------------------
Enhancements indicated by the above workaround:
1) The starting angle of a helix ought to be based on something tangible and
intuitive, like the Horizontal orientation of the sketch used to define the
Helix. Since that is not used, I can't quite fathom what reference is
defining 0 degrees (any help from the group?). My enhancement request is
either
a) have the zero point of a helix's angular offset be set at the horizontal
of the sketch used to define the helix, or
b) have the zero point of the helix angular offset be something clear and
definable, and spell out what that is in the 'Help' menu for the helix.
2) The fly-out feature manager has to have all of the functionality of the
real feature manager. If I can double click an icon and get things to pop
up on the screen in the regular feature manager, I need to be able to do
that in the flyout manager as well. Once again, we need things to be
consistent in the interface, or the user base will collectively lose
thousands and thousands of man-hours testing out where these limitations
are!
3) We need to be able to link the values of a helix's angular offset to
other angular dimensions in our parts. Do I need to repeat consistency?
4) When I double click a boss extrude, I get the dimensions for the feature
and for the absorbed sketch. This behavior really has to be consistent
across all feature types - including helixes. When I double click a helix
today, I do not get the dimensions of the absorbed sketch. Why not?
Once again (again!), we need things to be consistent in the interface, or
the user base will collectively lose thousands and thousands of man-hours
testing out where these limitations are!
5) If the property manager is up because it is auto-enabled, and I split the
feature manager area, the area doesn't stay split when the property manager
gets checked off. However, if the feature manager is selected and I split
the design tree, it stays split. If the configuration manager is up and I
split the feature manager tree, it stays split. Why is this behavior not
consistent enough to include the property manager?
If I split the property manager, auto enabled or no, the area should stay
split from then on . The reason is obvious - if I feel the need to split
the feature tree when the property manager pops up, it stands to reason that
I will probably need to split it every time the property manager pops up -
its not like the conditions have changed or anything. If SW wants, they can
keep it unsplit when it auto disenables (or whatever the word would be). It
just has to return to a split when it auto- enables, if I have already
indicated to the software that this is how I want it
6) We really need to be able to tear off a section of the property
manger/feature manager and park it somewhere else on the screen. With SW
cramming all sorts of functionality in this one area (dialogs, features,
etc), we are developing all sorts of inefficient conflicts. We need the
option to get around these conflicts by tearing off a section that we can
use as we will.
Regards, and good luck
-Ed
"Ilker Uludag" <iul...@umtas.com.tr> wrote in message
news:%GCI6.7947$ep.7...@e420r-atl1.usenetserver.com...
Thilo Trautwein
Good question.
A stupid answer would be: Because that's not how the function is set
up in SW.
There could be an workaround with an intermediate step, but with SW2K
you cannot drive the starting angle of a helix through an equation or
by hooking it up to an other dim (or to a point which has ref. dims in
your case) because it's not exposed by SW. I think this problem was
mentioned a good while ago, but I'm not sure anymore.
While at that subject, has anybody found a way to project a helix onto
a tube-like surface (varying diameter, not necessarily round)?
Are there any improvements for helix functions in 2001?
Thilo
Thilo Trautwein
John Picinich
127) in the new SolidWorks 2001 "Advanced Part Modeling" training book.
It uses a revolved surface and a helical path to create a swept surface that
uses the helical path as a guide curve.
The intersection curve command can then be used to create a helical curve
that follows the revolved surface.
Contact your SW VAR or purchase the latest training books for more details.
John Picinich
www.cadimensions.com
"Thilo Trautwein" <use...@acesgmbh.de> wrote in message
news:s2ucft4k5rdaoem65...@4ax.com...
Thilo Trautwein
<jo...@cadimensions.com> wrote:
>There is an interesting example using "Intersection Curves and Splines" (pg.
>127) in the new SolidWorks 2001 "Advanced Part Modeling" training book.
>
>It uses a revolved surface and a helical path to create a swept surface that
>uses the helical path as a guide curve.
>
>The intersection curve command can then be used to create a helical curve
>that follows the revolved surface.
>
>Contact your SW VAR or purchase the latest training books for more details.
That sounds great, finally something which justifies installing 2001
for me.
Thilo Trautwein
try. However, it seemed it still has the same problems as 2000 (and
all other versions before) when making "long" helical cuts.
The goal here is to cut a "thread" with the core diameter not being
constant along the length. It should be clear when looking at the
feature names.
SW apparently has two problems with it:
1) When you use only the core path as path for the cut, the profile
get's tilted and the cut then fails
2) When you use the outer ("cylindrical") edge of the helical surface
as path and the core path as guide curve, it goes down nicely all 34x
sections, except the last one. This jumps up one pitch and then of
course messes up the cut function.
I don't have access to the manuals mentioned below, but I think they
show what I'm trying to accomplish in my file. I'm pretty sure you can
do this with a smaller length/diameter ratio, but this is not of much
help when you have to show longer parts.
If somebody has a few minutes to mess with it, here is the file
(252k), SW2001:
www.acesgmbh.de/Challenge/ScrewBug2.SLDPRT
I tried to keep it simple, however I would like to be able to do this
with more changes in the diameter or even non-round core diameters
(elliptical, rounded squares) as well once this is fixed.
I particularly invite SW to take a look at it and ask them to fix it
or show an alternate method for the problem with the same dimensions
used as in the file.
Thanks,
Thilo Trautwein
On Mon, 14 May 2001 14:45:56 GMT, "John Picinich"
<jo...@cadimensions.com> wrote:
Jerry Steiger
> After reading some interesting comments about 2001 I finally gave it a
> try. However, it seemed it still has the same problems as 2000 (and
> all other versions before) when making "long" helical cuts.
Thilo,
I haven't loaded SW2001 yet, so I can't open your file yet, but I seem to
remember someone advising that the algorithms for helices aren't very
accurate and that they work best if you break a long helix into a number of
short sections. Would that work for you?
Jerry Steiger
Thilo Trautwein
I could use this in some simple cases, but it's ridiculous because it
means an effort of several hours for a single feature to work which
should take no longer then 2-3 minutes to set up. I would need
equations, several helices, surfaces and curves and still you have to
be afraid it will fail in a different configuration with a different
length. In real life it's no solution for me.
A helix can be precisely defined and it's not even very complicated to
do. The parasolid itself is capable of doing it because a colleague
can do the same thing in Unigraphics with two helices and a law curve.
Thilo Trautwein
Scott
I looked at your file. I have never messed with surfaces before, but plan to
try them in the near future. I did manage to get it to work by changing the
dimension #'s to 1.5 & 2. It really got weird after it made the slope. I
will have to look at it at home to get a better feel for it. I don't have a
lot of time right now to take it apart. But I hope someone can help you out
quicker than I can.
Sorry,
Scott
"Thilo Trautwein" <use...@acesgmbh.de> wrote in message
news:4i72gtodak48d0pbm...@4ax.com...
Thilo Trautwein
from past experience you have to use a second helix whenever the
diameter changes. Use one cylindrical helix as sweep path and the
second as guide curve to modify the profile (control the distance to
the center). This avoids the potato chip problem.
In my example one could use the outer edge of the helical surface as
"cylindrical" sweep path and the combined curve as guide curve. When
you preview the sections it all works perfect until the very last one,
which jumps around. If SW could fix this I believe most helix-problems
would be solved.
Thanks for your time!
On Tue, 15 May 2001 18:39:10 GMT, ken_bos...@porex.com wrote:
>Thilo,
>
>I was able to get the sweep to cut successfully by changing the
>thickness of the thread from 1.8 to 1.5. Unfortunately after the
>transition from the tapered end of the helix the straight part of the
>thread looks like a potato chip ;/ Probably not the results you were
>intending. I'm guessing that you would have to create a second helix
>to use as a guide curve to keep the thread form from distorting.
>
>Ken