Did Solid Works forget about Drawings?

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

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?

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?

Ed wrote:

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:

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.

Ed 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.

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

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:

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.