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
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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

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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?
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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.
bill allemann wrote:

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bill allemann wrote:

I thought that was why they began including DWGEDITOR with SW now.
-
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j wrote:

Oh yeah....like that's stable too.
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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
Dave Nay wrote:

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Diego wrote:

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
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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
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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?
Ed wrote:

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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.
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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.
Ed wrote:

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TOP wrote:

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.
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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

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Devon T. Sowell wrote:

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.
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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

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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.
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ick wrote:

Very interesting.... the old DXF trick. I think that we used to use this technique ACAD or Cadkey? I will give this a try too... thanks.
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Devon T. Sowell wrote:

Excellent! I will give this a try. Thanks.
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I totally agree.
-DWH
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