Did Solid Works forget about Drawings?

I continue to run into strange things and buggs with I make SW
drawings. Here is some of my current experience:

The project is a series of parts with truncated stub ACME threads which
are on a few degrees of taper, ( I know, this is a strange thread).
When I went to model such an unusual arrangement, it was relatively
easy to make the model. However, when I went to make a dimensioned
"detail" of the thread I ran into a number of problems:

The first was because the surfaces were all rouned and at strange
angles the dimension tool could not "grab" any surfaces, (or edge of
surfaces). I do not believe that this should have been much of a
challenge because to me a 2D view of a 3D part should be a FLAT 2D view
of the part and the edges should be nothing more then lines in the 2D
view. After a couple of hours of searching around, I found a reference
to using the "intersecting curve" tool, (found in the Sketch tool bar).
This worked fine but the dimension tool still would not grab onto any
of the edges/ points. I finally was able to project the intersecting
curve sketch using the "convert entities" onto the drawing plane which
the dimension tool finally was able to make connections. But, this was
not an easy process and definately not intuitive.

The second problem was that I didn't want to go through all of the
trouble repeating the above procedre a number of times. So, I thought
I would just make a copy of the detail. However, to make a simple
"detail" was also not as easy as one would expect. I tried cut and
pasting, making a block, and deleating the previous views so that I
could copy the drawing with a new drawing number, (leaving the old
detail in tact). But, none of this worked. Am I the only one that
uses standard "details"? Of course this is the purpose of blocks but
the block function absolutely would not accept the geometery!
Apparently because the geometery was referenced, (ie. by a detail view)
the block function could not recognize the geometery. Again, if the
views are representative of the parts, (ie. flattened) there should not
be a problem. I then attempted to delete the previous views, leaving
only the detail view but this wouldn't work either. Apparently detail
views and and section views have some sort of an unbreakable link to
the previous view, (at least I could not find where to break such a
link). I ultimately hid the previous view and placed the various parts
on top of the hidden view.

Again, all of this could have been easily solved if there were a
"flatten" command. In such an attempt I tried to save the drawing as a
"detached drawing". Which also didn't work.

The thing is that I have ran into problems with drawings that I would
consider to be fairly simple tasks fairly often. Does anyone at SW
every use this software. Apparently they do when it comes to modeling
but probably not drawings. I have also sent in bugg reports and some
fairly obvious things just don't seem to get addressed.

I am still using ACAD R14 for schematic drawigns because block move and
stretch are such basic commands. There really isn't any reason why SW
sketch shouldn't have these features as well. The whole idea around
sketches is that one can "free hand draw" a sketch and then start
placing constraints and dimensions later. A big part of making the
origional sketch should be the ability to block move and stretch,
(quick and easily) portions of the sketch around. Not having such a
basic command really makes me wonder.

Here is another basic feature missing. This is the concept of being
able to select specific features while in an assembly for making
measurments. The filtering tool attempts to fill in this void but I
find the filter tool to be very tedious to use. Probably mostly
because the filters stay on while in previous CAD programs the filter
was only valid for one selection while in the measurement mode. But
features such as center point of an edge, center or quadrant of a
circular edge, etc. are very important when making some measurements.
These tools are available in sketches etc but not in the assembly.
There have been times when the assembly measure tool just would not get
the critical measurement that I needed. As a work around, I made a
sketch, converted several edges where I could actually make a
measurement to some of these points. But, this is very tedious
compared to just making a measurement between two 3D points. The funny
thing is that certain things can be "grabbed" with the measurement tool
and filters, but, apparently someone decided that no one would ever
need to use some of the other types of points. These selections points
are available in the sketch environment? Just how does someone decide
that some points are important while others are not?

Is this just me? Or, are there some simple solutions to these issues?

Thanks,

Ed

 

Hello Ed-

Have your tried Insert Model Items, Dimensions? This will insert the 3D
sketch Dimensions from the model into the Drawing. Look in the Help file for
more information.

Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

To answer one of your questions...
No, I don't believe that swx personnel use the software outside of doing the
show demo performances, and even that is limited to modeling.
When it comes to drawings, I don't think that they even have face to face
contact with users on any regular basis.
If they did, how could so many bugs and time wasters stay in the software
for years?

news:...

 

Ed -

It sounds like your needs are rather abstract - needing to do drawings
and high level stuff like that. I find your whole idea of needing to
make drawings a bit strange. Why on earth would you even need that
stuff anymore? Maybe you need to look into making the screw threads
with some sort of rapid prototyping method like stereo lithography -
nobody needs drawings for that process and neither should you.

I find it absurd that you would want a high powered modeler like
solidwerks to handle something as mundane as drawings well. Come on -
the guys who wrote this stuff don't really use drawings that much and
they are happy.

Hahah - I agree with you - the whole drawing environment is "spongey"
and not really the best for getting real work done quickly, especially
when a projection of what should be a line or arc is coming through as
a spline and hence unselectable. Autocad will not let you dimension
splines either, but if something is a pain, you just redraw it as a
line and get on with life. A too like autocad for the straight forward
way in which I can detail anything any way I like with not so many
encumbernaces. With solidworks sometimes its like trying to tie your
shoes with chopsticks.

Ok the short awnser is that you have to live with it. Oh yeah, so do
the rest of us, so you have many people who sympathize (grin).

Take care -

SMA

 

You might want to attend a SolidWorks Drawings Essentials class. Other
than drawing 2x4s I can imagine SW being slower than ACAD. SW always
tries to make correct projections of objects. In 2D CAD it is up to
the draftsman whether the projection is correct or not. Many times 2D
CAD will simplify to make speed.

As far as picking edges to dimension on your ACME thread you might want
to describe how you made it. It is possible you set yourself up for
problems when you made the part. We're here to help you past that.

I am guessing you made the thread with a sweep. Describe the generatrix
(profile) and directrix (sweep curve). The profile should be kept
simple. Any fillets or rounds should be added after the sweep.

Is the sketch plane for the generatrix perpendicular to the directrix
or does it contain the axis of the thread? If the generatrix plane
contains the axis can you arrange for it to be in a position convenient
for creating a drawing view later?

Is the crest of the Acme thread parallel to the axis of the thread or
does it follow the taper?

 

Bill,

I'll have to disagree there. I have been in SW seminars at the Racine
SW show and at SWW. There are a couple of guys that really stir the pot
and get user input. And the users don't need much stirring. It is
usually a free for all.

That being said, I sometimes think SW should have left drawings as an
addin for a third party to come up with.

 

Wow! Some great comments. I will attempt to answer some of the
questions:

1) Comment: "Have your tried Insert Model Items, Dimensions? This will
insert the 3D
sketch Dimensions from the model into the Drawing. Look in the Help
file for
more information."

Answer: Yes, but the results were not much help.

2) Comment: "I am guessing you made the thread with a sweep. Describe
the generatrix (profile) and directrix (sweep curve). The profile
should be kept
simple. Any fillets or rounds should be added after the sweep. "

Answer: I did make the thread with a profile and a sweep curve as you
guessed. The profile is fairly simple but the surfaces of the thread
are at specified angles. The thread itself is also on a few degrees of
taper. There are no fillets or rounds. SW did a great job of modeling
this unusual thread, but it was just about impossible to actually
detail it.

3) Comment: "Is the sketch plane for the generatrix perpendicular to
the directrix
or does it contain the axis of the thread? If the generatrix plane
contains the axis can you arrange for it to be in a position convenient

for creating a drawing view later? "

Answer: I think what you are asking is that when the thread exits the
end of the part, is there a good representation of it in a standard
view. The answer is no because of the compound angles interfacing the
end of the round part. I had to create a plane, (that could be used to
define the view) that was generated with the axis of the part and a
line through the center of the part to the high point on the thread,
(just before it exited the end of the part). All of this was a fair
amount of work which is why I didn't want to keep duplicating this for
each part. Of course I only discovered that I needed all of these
extra planes etc. after the base part had been copied several times.
But I have ran into this before where I need to make a "detail" that
could be used on a number of drawings.

4) Comment: "Is the crest of the Acme thread parallel to the axis of
the thread or
does it follow the taper?"

Answer: It follows the taper.

It just seems like a 2D representative, ie. flat sketch, (in a 2D view)
should be an option.

Probably the biggest thing that concerns me is that SW is up to 10+
versions and some fairly obvious things still have not been addressed.

Hopefully, if we mumble about this enough that someone at SW will start
to get some drawings improvements.

 

Let's approach this question another way. I have cut Acmes before. I
use a tool ground to the appropriate form and angle held in a tool post
of a lathe. If you imagine the full triangle formed by the truncated
cutting tool pointing at the axis of the turning part it should define
a plane that includes the axis of the part. The tool rides up and down
the part along the axis of the part on ways that are parallel to the
axis of the turned part. Therefore the view plane showing the sides of
the thread is going to be parallel to a plane containing the axis of
the part. If I was cutting a tapered Acme I would taper the part first
and cut in the thread later. The tapered surface is simply a cone and
is easily shown on a normal drawing view.

If you are really trying to dimension the profile where a thread exits
a part I would have to ask why? This is not only going to be difficult
to draw but difficult to measure. A section view should show the true
profile for a normal thread.

Maybe I'm missing something about how this thread will be made.

 

This specific situation with the thread is really an example where it
is fairly easy to create a 3D model but extremely difficult to document
in the drawing environment. One would hope that by the time 14 or so
versions have been released that such issues would have been resolved.


More specifically, the dimension of the roots and lands of the thread
are not equal and need to be displayed. The angle of the leading and
trailing edges of the of the threads are also not equal and also need
to be displayed. It is pretty hard to place a dimension when the
dimension tool will not "recognize" the features in the 2D drawing.
This just should not be a problem.

 

I thought that was why they began including DWGEDITOR with SW now.

 

Oh yeah....like that's stable too.

 

Hello Ed-

RE:"It is pretty hard to place a dimension when the
dimension tool will not "recognize" the features in the 2D drawing.
This just should not be a problem."

Have you tried this? In the 3D model file, create a Plane Normal to the Edge
you want to show. Then, using the Convert Entities Tool, select the edge and
create a Sketch on this new plane. Show this sketch in the Drawing View and
dimension this Sketch.

Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

Very interesting topic, but it sounds like a very expensive part to
make as well.

I'm just curious about the application. What's it going into and why
such an unusual profile?

Diego

 

Drawings have always been a weak point in SolidWorks, but they are never
improved by trying to use SW in the same way you might have used Autocad.

SW has a hard time making a dimensioned drawing of a complex shape, but
that's no surprise. Acad could make a dimensioned drawing, but it would
only be an approximation of the shape.

It comes down to how you're going to manufacture the part. If you're
going to give someone a 2D print and have them make the part on a gear
hobbing machine, then use the Acad approximation, because the geometry
shown on the paper print doesn't matter, only a few feature parameters.
If you're going to work from the solid model to drive a CNC of some
type, use the model, and use a print for general reference.

I know to some people it's a sacrilege to say you can manufacture
without a paper print, but it happens all the time, especially with
complex shapes which can't be adequately described in 2D anyway.

It sounds like you need some basic training or to give up trying to make
SW work like Acad. Detail views should be easy enough, and there are
certainly ways to move or copy portions of sketches or entire sketches.
As for filters, there are hotkeys that make dealing with them a bit
easier. For measurement, maybe you haven't seen the numbers shown in the
task bar, which can show distances without even using the measure tool.

Good luck,

Matt

 

Because of proprietary reasons that I can't say a lot about the
application but apparently there is a machine that excepts these parts,
(as part of a process) and the machine manufacturer came up with this
"quick change" way of holding this tooling. The tooling is consumable
so the parts that I am detailing are changed fairly often.

I hope that this helps give you some idea..

Ed

 

For the most part I agree with your comments reguarding ACAD vs SW.
However, the reality is that the Client want's to standardize on SW,
(not a bad choice) and there are shops out there at every level of
capability from sketches on napkins to full 3D paperless CNC. But, as
desginers and consultants, unless we are so successful that we can pick
and choose what situations that suits our needs, (or CAD software) we
are pretty much stuck with trying to get SW to do what we need.

But, again, the point is and I suspect that a majority of the users of
SW struggle with aspects of the drawing environment that probably
should have been corrected serveral versions ago.

I appreciate your comments and my goal/hope is that if enough of these
threads keep going that SW may eventually take notice. The sad part
about the drawing environment improvements are relatively easy compared
to developing the "model" side of the package. This is a question of
priorities for SW and I for one believe that it is time to get the
drawing side cleaned. I don't know, perhaps not very many folks agree
with me?

 

Devon,

Thanks, your suggestion is exactly what I ended up doing. However, I
used an "intersection curve". When I actually got the curve and the
part into a view I still had to Convert the entities of the
intersection curve to the "sketch" of the drawing view. This just
seems like this was way more steps then should have been necessary and
I was still not able to make a block out of this so that I could make a
standard detail.

 

Hello Ed-

Once your have the Sketch you need, try this;

1. Break all External References in the Sketch, then redefine and dimension.
2. Save this Sketch as a Library Part.

Also, Sketches that are "shown" in Part and Assembly files don't always
"show" in Drawings;
a. In the Drawing, make sure View, Sketches is selected.
b. Then, in the Drawing, expand the Feature Tree to the Sketch, even though
its displayed as "shown", its not. Therefore, Right Click on the Sketch in
the Tree and select "Show".

Is this alot of work? Yes it is. But once you do it a few times, it goes
faster.

Cheers,
Devon

 

If you want to "explode" of "flatten" a drawing view to save as a
standard block:

1) save the drawing as a dxf
2) open the dxf file in SW NOT the dwgeditor (aka toilet-paper
software)
3) create the block from the resulting lines.

For better or worse, this method will break all references to the
initial files and geometry.

 

3D does give the capability of creating geometry that cannot be
projected true length on any plane. That kind of thing is not the
software's fault so much as it is the inability to flatten 3D geometry
properly. And that problem has been around since the silicon in your
computer chips was still on the beach Columbus landed on. It is
impossible to flatten a sphere and get true length lines. Many times SW
will not project the lines for dimensioning because they are not truly
linear or at least projected true length.