Drawing-Focused design in SW 3

[Sparweb]

Hi,
I'm still pretty new to Solidworks, but I am far from new to CAD, having spent the first 20 years of my career using AutoCAD and Inventor.
A year into the transition to Solidworks, I still feel shaky. I don't want to treat it unfairly, but I'm repeatedly hunting around for the workflows I'm used to, and clumsy picking up the new ones. That's all on me, but I'd like to improve.

One bias that I keep running up against is that Solidworks seems to be geared toward modelers, not drawers. While I do enjoy making an elegant model, I usually don't see the point of trying because I am thinking about the eventual drawing that will be produced. I often know that the end product - the drawing - will require very little detail in the model to be an accurate drawing so I don't model things very finely. This may be peculiar to the area I work in and way I do things. But it often causes the following things to happen:

* My models are done very quickly
* My drawings are elaborate
* My google searches for Solidworks tips I need come up empty/irrelevant
* My searches of the help files turn up irrelevant things or "I can't do that Dave".

I personally think my workflows are much more economic than my coworkers. I regularly finish a complete set of work instructions in 1/2 the time they take. But now my unfamiliarity with Solidworks is slowing me down.

Can anyone recommend blogs or groups that are **DRAWING FOCUSED** like I am?

No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[Jboggs]

Have you asked any of your SW related questions here?

I started out on the board, before CAD even existed. Its hard to get more "drawing centered" than that. Then I ran AutoCAD for over 20 years before transitioning to Solidworks. I find it to be a very efficient way of producing a drawing with adequate detail to fully convey the design function and requirements.

 

[Jboggs]

After I posted above I did my own research and see that you have indeed asked some of your questions here. My advice would be to just keep on keeping on. After a year I was still struggling some too. Hang in there and you will begin to see some real advantages as you understand more and more about how SW does its work.

 

[SBaugh]

Sounds to be like you need to spend more time on your models and make them with finer detail. Then while in the drawing you can express those details as needed with your views, details or sections. I didn't spend much time in the 2D CAD world after college. Shortly after getting a job that was using ProDesigner they moved to SW (1995) and I have been using it ever since. While at College we were using CADDS5 so I have been doing far more 3D modeling then drawing. However, with that said we did spend a large majority of our time learning on the board versus a computer. So Drawings are a large part of who I am and I understand drawings very well. I have done some very elaborate and complex drawings over the years in Solidworks.

What do you feel is missing in SW that you cannot make elaborate drawings?

This is why I think its the quick modeling that is causing you the problems that you are seeing.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[ctopher]

Have you had any SolidWorks training? If not, I strongly suggest it. It would help to switch from the ACAD mindset to the 3D SW mindset, different world. It would benefit you.

Chris, CSWP
SolidWorks '17
ctophers home
SolidWorks Legion

 

[SBaugh]

Here are a couple of pages from my recent assembly build for our shop. It's not elaborate like some of the drawings that I have in my portfolio, but it gives you an idea. Check out on page 4 of the PDF, I added colors to the lines so they can be understood by our shop guys.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[TheTick]

Sparweb: What is it that you actually do? Drawings? Work instructions? Documentation?

If you're just kicking out drawings and WIs, it seems that the design and modeling should already be done somewhere. It seems off that one needs to create a fresh model for a WI.

Also, consider your position within the whole ecosystem. Who uses your information? Where do you get your information from? Who are your customers?

 

[Sparweb]

You're right. Some introductions are in order. I've been here for a while but I don't offer much detail about my daily workplace. Not that there's much that I can say - proprietary and at times restricted data are the rule - but it's not hard to find some examples online and even some used on Eng-Tips before.

Below is a typical drawing like one that I would make. On aircraft the CONTEXT IS EVERYTHING because systems like these are being installed in particular locations, fitting into tight spaces most of the time. A hole off by 0.05" can mean the difference between a good install and a repair to a part worth a quarter-million dollars. I would like to be making drawings at this level, as I used to be, in a different CAD system, but struggling in Solidworks. Notice, for example, the detailed call-outs on each leader. While I would prefer to use balloons rather than text labels, to each his own. Neither seem convenient in SW, but searches on the subject do not seem to help. When I sat down to learn how to do it in Inventor (8-ish) years ago, it was "obvious".

The drawing sample below also lacks some finesse, such as presenting surrounding structure in phantom lines. I am not finding techniques that allow this to be done conveniently in SW. Again, completely unable to find training material or even search terms that would allow me to express what I'm trying to do.

What do my models look like? See below for a taste. Not mine but very similar.

Models I use often have 10,000 parts to fling around. Some of the parts are in a new system being installed, and many others are just "there" to show where the new parts are supposed to go. If you were modeling this, you would want the new parts to be sufficiently detailed to accurately represent their assembly. If we are manufacturing the parts, then they're as detailed as they need to be to represent all of the features to be fabricated. On the other hand, the surrounding parts just have to be there to display the shape and position of the surrounding structure to which the new system is attached. Those parts need no more detail than the drawing needs to see.

To make enormous assemblies smoother, I reduce them to a few thousand or few hundred by use suppressing what's unnecessary. The underlying assembly has to open at least once so that I can isolate the parts needed for the job at hand. All I need is the CONTEXT to do a system routing, perhaps spanning the entire length of the airframe. Other times I may be cutting apart a number of those frames, or hanging new stuff from them. I am not having any trouble at all with this part of the transition to Solidworks. Models are easy in SW and relatively intuitive. That part of the transition has gone well. And I've always had the impression (maybe not accurate) that Solidworks is geared for models more than drawings.

I emphatically do not model things like these:

They have artistic merit, but I don't care. Since 90% of Solidworks advertising, feature growth, and training material seem to be aimed at modelers, not drawers, I am having trouble staying tuned in to anything on the official Dassault channels.

 

[Sparweb]

Sbaugh,
That's a nice example. Not quite the style I use, but I do like it. I don't get to use colours. I never put scale on iso views.
Usually I emphasize the "new" part with thick solid lines, and fade the "surrounding" parts with thin phantom lines. I also don't to explodes to often, but when I do, most of the parts are pieces of the subject assembly, so I wouldn't need to play with line styles in an explode, anyway. I haven't done an explode in Solidworks at all, yet.

Questions:
Are the item balloons used in the notes block "live" or just manually typed in?
Do you ever include a hierarchy in your BOM's?
Do you ever include vendor names, material types, or other such columns in your BOM's?
Do you spell "Radiator" the same way I do? (I am a pitiless checker!)


Coming back to my original subject, and hopefully addressing a few questions that have been asked. I hope I haven't given the impression that I avoid modeling to draw sketch lines on SW drawings all the time! Sure I use lots of sketch blocks with attributes, but that seems to be good practice and I'm expanding the library at the workplace now.

Where does one find resources to maximize one's use of the drawing tools in Solidworks?

Some subjects that involve drawings that I would like to learn about:
[ul]
[li]View preparation, orientation[/li]
[li]Section, crop, breakout view generation tool control[/li]
[li]Line formatting and styles[/li]
[li]Setting default fields in view titles[/li]
[li]Nested/stacked assembly hierarchies in BOM[/li]
[li]...and making all of this consistent with templates...[/li]
[/ul]
..for a start.


No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[Jboggs]

My first impression is that you need some good basic SW training. Are there co-workers there with more experience? That may or may not be a help. I've seen most designers just "do things the way they've always done them" even if their methods involve many more steps than required. They just don't have enough interest or curiosity to look around, investigate some different options, try some new things. Most folks don't seem to be curious about "I wonder what that button does?" or "What does that term mean?".

I would bet there are easier ways to accomplish many of the things you want to do. SW has lots of built-in "intelligence" available, if you know where to look for it. For example, I often use links to file properties in notations.

You can create custom properties and that opens up other options. For example, the production machines I design for my employer are built by outside firms. We expect them to purchase most commercial items as part of their scope. Sometimes there are some very expensive or proprietary items that we will provide. I added a custom property to the part template file that we use to show when a part will be provided by us. Then added a column in the assembly BOM template and linked it to that part property. So now the machine builder has a direct indicator of what parts we will provide to him.

There are also direct controls for line formatting and styles (Options, Document Properties), as well as all the other topics you mentioned. Spend some time in training, research, and as you have done in the past, asking questions here.

 

[SBaugh]

Thanks for replying Sparweb... let's see if I can help you or further confuse you.

Questions:
[li]Are the item balloons used in the notes block "live" or just manually typed in?[/li]
[li]Do you ever include a hierarchy in your BOM's?[/li]
[li]Do you ever include vendor names, material types, or other such columns in your BOM's?[/li]
[li]Do you spell "Radiator" the same way I do? (I am a pitiless checker!)[/li]

1) All the ballons are dynamic if they change the notes update. that is parametric technology 101 -
2) Hierarchy - I assume you mean indented BOM, where a Sub-assemblies lists all the parts within. Yes I do, mainly for our shop guys, not customers
3) Yes but it's not always required since my BOM's are not always directly used with our local software for ordering parts, etc...
4) Yes, I spell it just like that

Some subjects that involve drawings that I would like to learn about:
[li]View preparation, orientation[/li]
[li]Section, crop, breakout view generation tool control[/li]
[li]Line formatting and styles[/li]
[li]Setting default fields in view titles[/li]
[li]Nested/stacked assembly hierarchies in BOM[/li]
[li]...and making all of this consistent with templates...[/li]

1) View prep IMO takes place in the model. However, with that said you can always change your orientation. When you do that means your XYZ will not be in the oreintation you want or need it to be in. If that is the case then it is a must for you to know exactly how you want to layout your model from the start. For me, XYZ is not an issue as long as my model is in XYZ and not in some complex obscure angle I can't find.

2) Check out the Help\online tutorials it should all be right there. I personally use a lot of crop views in place of section views sometimes.

3)You can find line formats under the Line format toolbar. You can make custom lines as well. I have never needed to use anything more than what SW comes with but I know it is possible.... however after writing this I could not find anything within SW 2019. I did find this help article per 2018 -

https://help.solidworks.com/2018/English/SolidWorks/sldworks/HIDD_OPTIONS_LINE_STYLE.htm

[highlight #FCE94F]4) I don't follow you on setting Default Fields... are talking about having a drawing template saved with predefined views?[/highlight]

5) Check out Indented BOM's in the help.

6) Templates are your foundation and you can customize them as needed. I think that there are still going to be several items you are going to have to decide on as you make your drawing, such as which type of BOM to use. However, you can setup and create several different styles of BOM's. This is within your help and the online tutorials.

You might find it odd, but search and read through the help articles. I have been using SW since 1995 and I still read the help. No shame in doing that. I do think the tutorials will help, even if you have had some training. I think you mentioned you had some training, did that training include the drawing course? Most of the time VAR's just send that book home because there is never a lot of interest in that course.




Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[Sparweb]

Every once in a while...
... or far too often, depends on who you ask...
I say something snotty and this is one of those times.
Nobody in this office is as good at parametric CAD as me. In fact I haven't met that person yet (present company excluded).
Every time I take a classroom course, I break the software in ways that confuse the instructors.
I've done composite laminates, mechanisms, GD&T drawings, hydraulic system routes, hardware assortments, wood carvings and more with parametric CAD.
If you think my job sounds cool, well, we are hiring.
I gotta get back to work, so I can't reply in detail now, but I will as soon as I can later, since you have offered so many suggestions.
And I'll stop bragging, too.

No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[Sparweb]

...basic SW training....
Which usually goes "...blablabla... this is a title block, it's used to locate zones... blablabla... this is a Cut feature, it's used to make holes... blablabla"
No, I want advanced SW training.

Possible candidate

They expect you to take the "Essentials" course first. I will haggle with the resellers when they phone me (still waiting for them to call) about having to take this.

...You can create custom properties and that opens up other options. [...] I added a custom property to the part template file that we use to show when a part will be provided by us. Then added a column in the assembly BOM template and linked it to that part property. So now the machine builder has a direct indicator of what parts we will provide to him.

I tried to set that up, too, but something went wrong. I'll have to circle back someday to that subject to try again.

Which reminds me, more things on my list:
* Materials database; how to make custom materials.
* Document properties; adding fields

SBaugh,
1) All the balloons are dynamic if they change the notes update...
I am surprised... How can that be when there is no leader from the balloon to touch the object?
Those balloons show no association or link to a particular object. How does it determine the item number reference?
I'm on the cusp of discovering something that Inventor cannot do, just need a little more push...

"Indented BOM" kinda, but not quite.
Each assembly drawing in my industry tends to "create" a new assembly number using the part number - dash number combination in the BOM.
When I'm working on drawing 12345, and the first assembly is labeled -01 in the part numbers column, then the assembly's complete part number is "12345-01".
On such drawings I can (I DARE!) to put multiple assemblies, creating multiple assembly part numbers. Some assemblies nest into other assemblies, even. Now in the BOM you find more -02, -03 and so on, and that generates many separate assemblies with separate part numbers, all quite distinguishable from each other. All of my shop hands understand and expect this. I have not yet found a convenient way to generate such a BOM structure in Solidworks. I have to use lots of custom rows in the table. Nobody else in the office knows how either - I asked.
BTW Inventor was not good at this either - but we did have a macro that would set it up for you once you had the assembly views placed on it.

2) Check out the Help\online tutorials it should all be right there.
OMG
Nothing could be more mickey-mouse than this.



That link to search for more in the KB just leads to support tickets!!

Don't you use phantom lines?

I have some hope for figuring out Templates, but I won't try tackling that until I've mastered more of the basic skills/workarounds needed.

Default fields in view titles: Every time I place a view, the title under it is "SCALE 1:1". No thanks, that's one piece of information that I NEVER keep on my drawing view labels. Where is the Part Number and Part Description? All of my models have the p/n and description entered in the document properties, and they appear in the BOM well enough. Why can't this be put on the view title?


No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[tz101]

Some good SW training will go a long way. I will also add that a finely tuned model makes the drawing portion go smoothly and relatively quickly in SW. When working in any 3D CAD software, always considering the model to be the master is the best practice. I have mainly worked in Pro/E-Creo and SolidWorks and that has proven true in both cases. My 2 cents..

 

[SBaugh]

SBaugh, 1) All the balloons are dynamic if they change the notes update...
I am surprised... How can that be when there is no leader from the balloon to touch the object? Those balloons show no association or link to a particular object. How does it determine the item number reference? I'm on the cusp of discovering something that Inventor cannot do, just need a little more push...

The balloons that are in my notes are directly linked to the ballons from the assembly or the balloons per the views in the drawings. If you are editing the annotation or note text and click on the balloon it automatically and is directly linked to that balloon. If the item number changes for that part then the note balloon updates. If that part disappears so does the balloon in the notes, and your notes read strangely.

I have been known to add the assembly to the drawing sheet and link to those balloons and then hide the view.

"Indented BOM" kinda, but not quite.
Each assembly drawing in my industry tends to "create" a new assembly number using the part number - dash number combination in the BOM.
When I'm working on drawing 12345, and the first assembly is labeled -01 in the part numbers column, then the assembly's complete part number is "12345-01".
On such drawings, I can (I DARE!) to put multiple assemblies, creating multiple assembly part numbers. Some assemblies nest into other assemblies, even. Now in the BOM, you find more -02, -03 and so on, and that generates many separate assemblies with separate part numbers, all quite distinguishable from each other. All of my shop hands understand and expect this. I have not yet found a convenient way to generate such a BOM structure in Solidworks. I have to use lots of custom rows in the table. Nobody else in the office knows how either - I asked.
BTW Inventor was not good at this either - but we did have a macro that would set it up for you once you had the assembly views placed on it.

To my knowledge that is the extent of what SW can do with an indented BOM. It might be possible to do what you are asking if you knew how to write your own program using SW API.

Don't you use phantom lines?

I have some hope for figuring out Templates, but I won't try tackling that until I've mastered more of the basic skills/workarounds needed.

Default fields in view titles: Every time I place a view, the title under it is "SCALE 1:1". No thanks, that's one piece of information that I NEVER keep on my drawing view labels. Where is the Part Number and Part Description? All of my models have the p/n and description entered in the document properties, and they appear in the BOM well enough. Why can't this be put on the view title?


Yes, I use Phantom lines when it's appropriate.

I assume you want your fields in the drawing to auto-populate with Part number \ description? Click on the "link to the property" and select the "property". Such as "Part Number", "Part Description" etc...

If you have a drawing and a model loaded into the drawing and say something is incorrect, you can RMB the annotation and select "Edit text in window". There you can see the link text information to ensure you are pulling the correct property. You can also see how to write it into the fields manually, but you have to do it from the "edit text window".

As for your scale, you just don't have any of the drawing templates set up correctly or linked correctly. Understanding how drawings templates and how to link is not simple and takes time. You are going to spend a lot of time in your help and on here looking for your answers. I am sure your questions have already been asked on here from years past. Honestly, I don't think the basic function of SW drawings has ever changed. They have added several new items to drawings, but how it works and links is still the same.

Drawings have 2 layers to it. "Sheet format" (*.slddrt) is one layer and the other is the "Template" (*.drwdot) itself. Knowing that the template uses the sheet format and all its links, is half the battle.

If you have not done the essentials you really need to IMHO. Even though I taught myself how to use SW from 95 on when I went to work for a VAR (in 2002-2010) I took the essential course and I still learned a lot that I didn't know and a lot that I was not doing as efficient as I could be. I think SW will, for the most part, do what you want, but you have to get the training and build that foundation up before you start tackling the advanced stuff. In my opinion and from my past experiences... if you are battling with some of the basic functions of SW now, your going to be even further lost in the advanced stuff. People coming from AutoCAD have a much harder time making the switch and those that loved their ACAD usually don't make the switch. I worked for a company where I was the CAD Admin for over 200 CAD users of both SW, Pro-E, and ACAD. The ACAD users that wanted to use SW just had a really hard time grasping it. Not saying you can't do it, just my past experiences. I have seen ACAD users intent on Advanced training to end up going back to Essentials because they just didn't have the knowledge that was needed in the advanced training and ended up costing the company more money. Pro-E users and other 3D cad software people usually make the switch much easier.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[TheTick]

My sympathies, Sparweb

It does seem SW is not quite the right tool for the job (though I can't imagine how Inventor could be better). Seems more like a job for SW Composer.

The bridge between CAD and illustration has never been that firm.

 

[Sparweb]

Tick,
CATIA is the right tool for my job.
But my company doesn't have the cash!

No response yet from the two SW resellers I e-mailed.

I have suspected that the company templates are lacking some things. I probably shouldn't have shared my "pet peeves" with you, and stuck to the basic question.
Just gotta put in the legwork (mousework) to get where I want to go. I'm still disappointed that nobody could refer to any drawing resources other than the "help files".
My questions on the Dassault SW forum go unanswered. For example, this question has been there for a week.



No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[Sparweb]

SBaugh,
A quick thank you for a number of tips that I can use right away.

Going further with item balloons within a block of text... indeed I never found a way to to that in Inventor.
This could be very handy. Can I also cross-reference my way to the item's part number too?
Imagine being able to write:

​

"Apply adhesive [EC1367] to top face of [plate] [121212-03] uniformly using brush applicator."
...and link the name of the adhesive from the BOM and link the part name and number from an item reference. Then if the selection of adhesive has to change the reference in the note updates along with it!


No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF

 

[drawoh]

SparWeb,

I recently took a SolidWorks assembly model, and I created a document with assembly process instructions, nine pages long. It worked pretty well.

Item numbers are intelligent. You can click on them and add them to your notes. Everything updates intelligently. You can click on parts on the views and extract the descriptions intelligently. I like to define parts as assemblies if there is any change there will be pins and thread inserts. This messes up clicking for descriptions.

I did not use configurations to create the drawing views. I used the named displays and views. SolidWorks supports multiple exploded views.

I wish the text editor was smarter. I would like to parametrically refer to note numbers. I had to define each page with its own drawing views and separate notes. SolidWorks is not a word processor.

--
JHG

 

[Sparweb]

I used the named displays and views...

Do you mean the saved views in the model on the view toolbar? It never occurred to me that you could use them when placing/orienting views. I'll go look for how to do that. Thank you! I have a drawing on the go where I need that.

No one believes the theory except the one who developed it. Everyone believes the experiment except the one who ran it.
STF