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brothapig
08-08-2016, 02:29 PM
Can someone confirm that the free license through EAA (student version) comes complete with the toolbox and smart fasteners?
When I try to use them in an assembly, I get the message that the toolbox is not installed. When I try to configure, I get the "manage licenses" screen (maybe indicating I don't have the correct license?). My google searches are not conclusive.
Note that I CAN get to the "Hole Wizard" in the toolbox setup, but none of the others listed are clickable:

5681

Jeffrey Meyer
08-08-2016, 02:47 PM
The Toolbox is an add-in - not loaded by default.

Go to: Tools > Add-ins
You can activate the add-ins on a one-time basis or have them loaded every time you enter SW. The Toolbox is one such add-in.
I'm not sure it's part of the EAA benefit - I think it is but not sure.
If it's not, let me know which fastener you need and I'll mail it to you in STEP or ParaSolid format.
If necessary we can ask the forum managers to assign us a special EAA vault for storage of such standard parts.

AnnaWood
08-08-2016, 08:12 PM
I am not sure if the SDK includes the Toolbox parts. It appears that it is not included. Have not installed SolidWorks SDK yet on my home computer to confirm that.

https://forum.solidworks.com/external-link.jspa?url=https%3A%2F%2Fwww.solidworks.com%2Fs w%2Fdocs%2FStudent_Access_Product_Matrix_LB.pdf


You can download SolidWorks fastener files from McMaster-Carr. That is what we use for all of our fasteners. Never have used Toolbox.

Tom Gagnon
08-08-2016, 08:49 PM
No. EAA/Student Version comes with the functionality of Solidworks Standard as I understand it. This page (http://www.solidworks.com/sw/products/3d-cad/3d-cad-matrix.htm) shows what is included in various levels of license. The language is not entirely clear, as it's Marketing (**sparkles**).

You can, however, make your own. It's not that hard unless you intend to use every part imaginable, particularly if you know what you need.

A great place to download STEP files of common hardware from is http://www.mcmaster.com/ Their models are clean and reliable in my experience, requiring no Import Diagnostics to fix them up. Edit: Most parts from McM are actual parts with feature tree intact, whereas I was confused with other vendors' downloaded files that I deal with more often.
(If you get one), The STEP isn't by default an associated file type. I import STEP files by dragging the file into a window of Solidworks that has no files already open. Edit: Step files import as a part without features, but imported bodies instead.

With the part saved to your Design Library in a "Fastener" or "Hardware" or other sorted directory, you can define SmartMates as a Reference Geometry Feature so that it seats into a hole (bolt, rivet, etc) or onto a bolt and seated to a surface (nuts) or what works for you in your workflow.

The Toolbox parts, specifically, will not load properly even if given to you because the add-in is not loaded. The only thing I find useful in the toolbox over parts which I've made myself as above is the automatic sizing of fasteners to the hole or bolt being placed upon. Furthermore in brief, some users have had bad experiences with Toolbox parts over the years between different releases, and have decided instead to keep their own instead for long term stability. Selecting the part from ordered lists can be just as simple, and also has better control over custom properties of each part, if SKU numbers are used.

Jeffrey Meyer
08-09-2016, 03:22 AM
My 2 cents worth:

1. I suspect that the vast majority of the EAA members who are going to use SW will do so for a few one-time personal projects, and they almost certainly won't need all the "automation" that comes with the Toolbox (SW or private) "smart" fasteners.

2. By definition the Toolbox contains "standard" components - i.e. you cannot change them - by definition. As such there is no point in downloading them to include the feature/history tree that only (unnecessarily) loads the your computer. In this case the feature/history tree is in fact a disadvantage because if you go to the trouble of defining your own "standard" part, you then discover that you cannot buy it anywhere.

3. The STEP file format is an in internationally accepted and controlled standard for exchanging data between CAD systems, while ParaSolid/DXF/PDF (et al) files are de facto proprietary standards with limited (if any) commitment to continuity.

4. STEP files are therefore the best way for you to import and build your standard/private "toolbox", and for your own private SW projects the ROI in converting your library to "smart" components, is highly dubious. (Maybe interesting if you're going to model and insert 20,000 rivets in your SW assembly of your RV:D.)

My 2 cents has become 4 cents:P

brothapig
08-09-2016, 07:22 AM
Well, it sounds as though I at least have an answer.
So, the student version obtained through EAA does not and will not/can not utilize the toolbox as it relates to fasteners. At least I can stop trying!
I played around a bit with some of the options discussed here. I downloaded a fastener from McM (STEP format), opened it in SW, saved as a part, and was able to add as a component in an assembly. It appears, however, that there will be no changing this part as far as length, thread, etc. after insertion; and any desired changed will require the import of the actual correct fastener.

Does this sound correct?

Jeffrey Meyer
08-09-2016, 08:35 AM
Well, it sounds as though I at least have an answer.
So, the student version obtained through EAA does not and will not/can not utilize the toolbox as it relates to fasteners. At least I can stop trying!
I played around a bit with some of the options discussed here. I downloaded a fastener from McM (STEP format), opened it in SW, saved as a part, and was able to add as a component in an assembly. It appears, however, that there will be no changing this part as far as length, thread, etc. after insertion; and any desired changed will require the import of the actual correct fastener.

Does this sound correct?

If there's one thing I've learned in life it's that the answer "no" is much better than the answer "don't know" (pun intended) - This is because the answer "don't know" leaves you in a state of uncertainty, while "no" lets you get on in life.

Philosophy aside, changing a part as far as length is concerned is quite easy: If it's too long, cut-it dear Henry, cut-it (as the song goes). If it's too short, extrude it dear Henry, ... The biggest benefit of the STEP file is that it contains the most difficult part of the fastener geometry as specified by the appropriate standard. For example, an M10 Cross Recessed Cheese Head screw has the same head geometry for all the thread lengths - You don't need to import a separate STEP file for each.

AnnaWood
08-09-2016, 04:49 PM
Well, it sounds as though I at least have an answer.
So, the student version obtained through EAA does not and will not/can not utilize the toolbox as it relates to fasteners. At least I can stop trying!
I played around a bit with some of the options discussed here. I downloaded a fastener from McM (STEP format), opened it in SW, saved as a part, and was able to add as a component in an assembly. It appears, however, that there will be no changing this part as far as length, thread, etc. after insertion; and any desired changed will require the import of the actual correct fastener.

Does this sound correct?

Yes, you will want to download the new correct fastener size with the correct part number from McMaster. You have the option of downloading native SolidWorks files as well. You are not limited to step files. Try that out as well to see what you prefer. To me it is easier to download a new file with the correct part number then copy file, rename the file and then modify to the correct size.


You can also make your own generic fastener and start building you own library. Here is Dropbox link to a generic model that we use for fasteners. Copy the file and change the file name for a new size fastener and edit accordingly.

https://www.dropbox.com/s/2oz6jhqdgp3a0kq/SHCS%20-%2010-32%20x%20.50%20Lg.sldprt?dl=0


We use the Holo-Krome Socket Screw Selector Chart for the model dimensions for our generic models.



https://www.amazon.com/Holo-Krome-Socket-Selector-Inches-99013/dp/B00EOHPBNG/ref=sr_1_1?s=industrial&ie=UTF8&qid=1470782803&sr=1-1&refinements=p_4%3AHolo-Krome
(https://www.amazon.com/Holo-Krome-Socket-Selector-Inches-99013/dp/B00EOHPBNG/ref=sr_1_1?s=industrial&ie=UTF8&qid=1470782803&sr=1-1&refinements=p_4%3AHolo-Krome)

There is no such thing as one right way to create your fasteners in SolidWorks. Find a system that works for you and then be consistent with it.


Another consideration is aircraft hardware is manufactured to AN hardware standards for sizes. Good plan is to get a hold of AN hardware size specs and create models to that if you are spec'ing AN hardware.

Jeffrey Meyer
08-09-2016, 11:20 PM
There is no such thing as one right way to create your fasteners in SolidWorks. Find a system that works for you and then be consistent with it.


Another consideration is aircraft hardware is manufactured to AN hardware standards for sizes. Good plan is to get a hold of AN hardware size specs and create models to that if you are spec'ing AN hardware.

Every word cast in stone.
I personally prefer specifying DIN metric fasteners - so much easier to understand for a pleb like me.

Hstaton
08-10-2016, 03:24 AM
Ok - so where at McMaster do you find these STEP files to download? I can't find a link on the site that I can download these from.

Jeffrey Meyer
08-10-2016, 04:56 AM
When you're in the McMaster site, choose the product that you want by drilling right down to the actual McMaster catalog number. At that point it will give you the option of downloading a 3D CAD file where the default file type is a native Solidworks file. You can of course use this SW file but you might find that your version of SW (student edition) may not be able to read it for one reason or another. So, instead of a SW file type download choose the STEP option - the student edition should be able to open it.
When SW asks you if you want checking or feature recognition, answer in the negative, and give it a few seconds to build the part. Save it.

Be aware that the McMaster STEP files produce very detailed geometry right down to the spiral threads on screws. If you have many screws in your design you might find that your CPU/memory gets bogged down, and your graphics processor works orders of magnitude more. While such detailed geometry is aesthetically appealing, IMHO it's not worth the degradation in performance of your computer. So, as I said before, cut it, dear Henry, cut it ...

Tom Gagnon
08-10-2016, 09:19 AM
Not everything McMaster sells has models to download, but for fasteners it covers all that I've experienced. Jeffrey is correct that you have to locate the part and then click on the CAD Drawing link with a crosshair center mark icon. That is, there is no site menu item for download area: it's ordered by catalog, then downloads are either available for that part # or not.

For threaded fasteners, I really prefer to download the Part so that I can suppress the thread cut feature. IIRC, it's usually a "Swept Cut" feature. It's nice that I haven't encountered any parts from there where subsequent features (in parent/children relation) rely on the thread being there. Otherwise, suppressing a parent will necessarily suppress its children. The part I find useful in assemblies at the scale I draw is a bolt with no thread shown as a cylinder with a hex head, a NPT (threaded pipe) socket expressed as a simple tapered smooth surface, etc. If drawing details with fasteners, you may want to unsuppress the features, which is doable with a part configuration in the part so you have a default and simple configs, or default and complex configs depending on what you'd normally use.

Either way, decide and establish a pattern that will be followed in your use for all fasteners as Anna pointed out very importantly: file naming, Description syntax, units, configuration names, names of references such as "Axis" vs "Axis1" or "Long Axis", even orientation on the origin & primary reference planes should all be consistent in your pattern. These things are important to make your task easier when using Replace Components (with mates) command in an assembly, sorting parts in a Bill of Materials, and much more. This is a difficult lesson to care about when starting out learning other basics, but once you learn more you may decide to rework all the bits you've gathered.

As a sidenote, beware of downloaded parts that are located far from their Origin. To me it shows that someone exported it from an assembly or a multibody part. Before saving or using any such part, I place the bodies onto the origin with constraints so it is more useful to describe relations in its use. I've never found McMaster to provide such boneheaded design parts, but the wider industrial market may choose to do things differently. (Example that comes to mind: Stahlin.com FRP electrical control panel enclosures.) Most often, if an item is modeled "on its back," that may be how it was manufactured, but not how it will be mounted to a wall or stand. It shows the manufacturer's design intent, not yours.

Another comprehensive online resource, if narrowly specific, is Swagelok compression tubing fittings. Their entire catalog is available in multiformat downloads, but again they like to place the origin on the end of a part, not say the central intersection of a Tee fitting.

Hstaton
08-11-2016, 03:52 AM
Thanks for the info on McMaster parts. I had forgotten about the link, because I never had software that could use it before! Now, my next dumb question refers to a comment made above about moving parts to the origin. I have been trying to determine how to do that and am completely stumped! How do you do it? Thanks in advance!

Jeffrey Meyer
08-11-2016, 05:51 AM
Like many actions in SW there are several ways to do this:

1. Go to Evaluate > Measure, on the body choose a vertex or center point that you want to be the origin of your part, and note the coordinates shown. Then go to Insert > Features > Move/Copy. Choose the body you want to move, and then as the reference point choose the point that you mesured previously. In the Translation boxes insert the negative values of the previously noted coordinates.

2. Go to Insert > Features > Move/Copy directly, choose the body you want to move, and then Add mates to the three main planes (or any other geometry) that are located at the target location.

3. If you have the history/feature tree then simply edit the first feature(s)/sketches so that they're located at your desired target.

There are probably more ways to skin this cat.

Jeffrey Meyer
08-11-2016, 06:08 AM
For threaded fasteners, I really prefer to download the Part so that I can suppress the thread cut feature. IIRC, it's usually a "Swept Cut" feature. It's nice that I haven't encountered any parts from there where subsequent features (in parent/children relation) rely on the thread being there. Otherwise, suppressing a parent will necessarily suppress its children. The part I find useful in assemblies at the scale I draw is a bolt with no thread shown as a cylinder with a hex head, a NPT (threaded pipe) socket expressed as a simple tapered smooth surface, etc. If drawing details with fasteners, you may want to unsuppress the features, which is doable with a part configuration in the part so you have a default and simple configs, or default and complex configs depending on what you'd normally use.


Here, here.
I did a small experiment in this regard: I took a beautiful McMaster screw and exported an STL representation (STL is the file type used by most 3D printers - breaks the geometry down into thousands of triangular facets). The number of facets came out at 54,876. I then removed the detailed thread as suggested by Tom, and the exported STL representation produced 1,764 facets. This is a factor of more than 30. That means 30 times more computation of the geometry, 30 times more graphics computation, and a great deal more storage/memory.
Thanks Tom.:)