It is frequently useful to verify that there is access for tools during the assembly of a product.
I am suggesting that you contribute your models of hand tools to this thread.
The attached model is a 3/8" (9.5mm) drive deep well socket with configurations for standard hex sizes from 10mm-19mm and 3/8" thru 3/4".
I thought for several seconds about donating this model to 3D Discontent Central. Since I seldom enjoy using that website and because I enjoy using this forum, the forum is the benefactor of this effort.
If you have suggestions for more efficient ways to model parts like this, I appreciate your feed back.
Message was edited by: Gerald Davis (used the apostrophe recommened by Depak to fix the underscore reported by Dale and added a "Create Property" manger to allow selecting of the size when inserting into an assembly and added a mate reference for concentricity)
I wouldn't have put the size labels on, but that's me.
I see one of the cells in the DT has a hyperlink in it. Do you know about the setting in Excel's spell checker that prevents it from turning everything with an "@" into a link? That drove me nuts for years.
If someone does extensions or any of the various drives, it would be nice to get some mate references working. That's the only real addition I can think to make.
I'm not clear why you would be opposed to uploading this to 3DCC too. One of its failings is gaps in the library, and this would be an excellent addition.
Another clean, efficient model. Where are you getting the dimensions from? IIRC, the data in MH isn't detailed enough for models this complete.
Looking at the design table again, I see you have all the dimensions named. Two questions come out of that:
I see you use underscore instead of a space in the dimension names. Have you found a place where spaces in dimension names are a problem or is this a defensive habit? I always wonder if spaces will be a problem. Custom property names, for example.
Do you ever rename sketches? I sometimes find it helpful when using design tables, because I can't remember what Sketch7 is, etc. I usually name the sketches after the feature, something like "skBody" for a sketch in feature "Body". For the second sketch in a HW hole, I use something like "profDowel".
...Have you found a place where spaces in dimension names are a problem or is this a defensive habit? Left over from my days using WordStar and CP/M. Spaces in object names used to really screw up software, so I avoid using them in labels
...Do you ever rename sketches? Yes, particularly when they are not absorbed. For example some of my electrical components have sketches for the board mounting holes. I'll rename those sketches accordlingly. Your suggestion for renaming the sketch for the benefit of equations and design tables has merit, too.
I make the models by (approximately) reverse engineering tools that I own. The dimensions are what I measure with my digital calipers and verify using various trade manuals and catalogs. These models may have a silly amount of detail (for example the ball detent groove in the drive pocket of the socket), but I also use the models when creating illustrations for instruction manuals and images for marketing.
Someone on 3DCC reported that the 17mm configuration failed. I corrected a selection for a circular pattern and updated the attachment both here and on 3DCC.
I see one of the cells in the DT has a hyperlink in it. Do you know about the setting in Excel's spell checker that prevents it from turning everything with an "@" into a link? That drove me nuts for years.
Just add a ' before you write a link and this will take care of them not turning into link.
There is a category for Hand Tools, Gerald. Doing a search for "wrenches" (autofill search) produces no results for your submission, but there are scads of others. Doing a search for "Gerald" pops up a Slam Latch with your name on it. If I select your name all of your models appear. Bit of a mess, really.
A mate references this time, eh? I dare you to make it fully mate with the socket when inserted into an assembly. Do you have the patience to pull it off without smashing your office furniture?
I renamed this one to "3-8 x 6 Extension" to be consistent with "3-8 Drive Deep Well Socket".
1) You should re-down-load the socket and the wrench - they both have mate ref's now.
2) Yes! Why aren't you adding your stuff? We need screw drivers, socket drives, hammers, pliers, crescent wrenches, etc. I have a set of nut drivers but the model is hiding from me at the moment.
3) Feel free to edit and repost variations on my stuff.
Here's a set of ball end hex keys in the inch variety.
Out of curiosity, is there a way to edit or even look at that design table if I only have MSExcel 2000?
My guess is that you should be able to open the table, but there may be a version limitation.
Try the following:
1) Click on the Configuration Manager tab at the top of the Feature Manager
2) Right Mouse Button (RMB) on the Design Table to see a context menu (see screen capture below)
3) Select "Edit Table" or "Edit Table in New Window" (the latter is my preference)
Excel should then launch and you're in control of the Design Table.
A 4th option is to select "Save Table" - that allows you to export it into a CSV or XLS format. If you do that, the spreadsheet you import/open with Excel is not linked to the model. That would at least allow you to examine the table.
It appears to address Office 2007>2003 but may not deal with 2000 - that's pretty anti-Balmer to keep using software that was distributed on 5-1/4" floppies!
That does not work either. I have the Microsoft compatibility tool installed on the computer I did the test on so I can open up the Office 2007 files I get. Even with the compatibility tool installed I can't open or save off the Excel 2007 DT with Excel 2000 installed.
For me, it is not an issue since we do not use design tables in our SolidWorks models. I also have other computers available with Office 2003 and Office 2007 installed that I can use if needed.
It appears to address Office 2007>2003 but may not deal with 2000 - that's pretty anti-Balmer to keep using software that was distributed on 5-1/4" floppies!
Anti-Ballmer? Who isn't?
But in this case, I'm just waiting (still) for IT to install a newer version of MSOffice.
I've given up, and don't really care anymore, so I've stopped pestering them since I use Thunderbird and OpenOffice for all my computing needs. I can even open the docx files that most people here still can't open. Heh. :-)
And I actually have a 5-1/4" floppy drive lying around somewhere at home. You know, just in case.
Out of curiosity, is there a way to edit or even look at that design table if I only have MSExcel 2000?
The best will be to save the DT as external excel file. You can open the hand tool files, delete the DT and reinsert it.
Well, here are the Design Tables in Excel 97-2003 format. To create these, I opened the design table in a new window and saved it as XLS. When you try to save the table directly from the drop down menu (screen capture shown in an earlier post) it will only save in the XLSX format.
To use the attached spread sheets, open the corresponding model, delete the design table, insert a new design table from the corresponding file.
I still want a way to save SolidWorks part files for backward compatibility - my dream is to run a tool that writes a macro that recreates the steps in the Feature Manager - including equations and feature names. Then the resulting macro is distributed. When the distributed macro is run on the target machine, the part is recreated in whatever version the target has installed.
Do you have any control over what format the DT is saved in when you made the DTs? Or does it default to XLSX?
If you do have control over it, could you do me a favor? Could you create a simple part and create a DT the same way you did with those tools? Trying to NOT use XLSX obviosuly tho.
I'm being told by my VAR that it's not a SW bug, but a problem where the object that is created is an Office2007 object, and therefore can't be opened or saved on a machine that does not have MSOffice2007 installed. So, I'm trying to understand the issue a bit better, and would like to know if the filetype matters.
If it does not matter, maybe SW should consider dumping the MSExcel requirement and creating DTs, etc internal to the program (tho obviously still with the ability to import XLS/XLSX, etc).
...Do you have any control over what format the DT is saved in when you made the DTs? Or does it default to XLSX?...
John -
I found this in the Excel help:
In Microsoft Office Excel 2007, workbooks (workbook: A spreadsheet program file that you create in Excel. A workbook contains worksheets of rows and columns in which you can enter and calculate data.) are saved as Excel Workbooks (.xlsx) by default. You can change the default file format to any other file format that is supported in Office Excel 2007. For example, if you frequently create macros in a workbook, you may want to automatically save a new workbook as an Excel Macro-Enabled Workbook (.xlsm). Or, if you work with others who use earlier versions of Microsoft Excel, you may want to save a new workbook as an Excel 97-2003 Workbook (.xls).
Click the Microsoft Office Button, and then click Excel Options.
In the Save category, under Save Workbooks, in the Save files in this format list, click the file format that you want to use.
I've made that change on my system to use xls instead of xlsx. Here's a sample part...
For whatever reason, SW still tries to save the DT as an XLSX, and I get the same thing as before where I go thru the whole save process but no file is saved. I can't edit the DT in SW either.
But, I do have Office 2000.
Anyone with MSOffice 2003 want to give it a shot? I doubt you'll see anything different tho.
John I have Office 2003 on my machine with file converter (to open 2007 version files) installed but that too doesn't work. Can't edit the DT made in office 2007 or even save it.
I have an incident open with my VAR, trying to get this labeled with SW as a bug. What I have so far is that the spreadsheet object is created in the Office2007 format, and there is as, as far as I am aware, no way to change that. It has nothing to do with the file format, but the embedded object.
I finally got around to working up a contribution, even though it's such a simple model. Just as I was preparing to post, I realized I could have simply edited the table for your model. Anyhow, here is a metric hex key. DIN 911 lengths, according to Maryland Metrics. The bend and the ball end are guesses.
Sorry about that. Here, I'll save them as a previous version...Oh, that's right...I can't. I don't believe I have them archived anywhere, but I'll take a look.
This might be good for discussion at user group meetings - boundary surface, derived sketch, twisted sweeps, split line, composite curve, surface thicken, virtual parts, path mates, motion study, sheet metal, revolves (speedy rebuild times), when is too much detail too much, variable pitch helix, limit mates, etc.
Perhaps the most important discussion is about the mechanical drawings and Bill of Materials - that's what all this modeling is for, isn't it?
The model has some merit - I'm fond of the handle. I'm going to suggest it as a model mania contest for our next user group meeting in Denver.
However, this assembly isn't really ready for manufacturing. That would take a bit more time to faithfully model the threads and verify interference points.
I'd love to see an animation that shows the grease pushing the check valves open as the handle is compressed and then see them reseat upon handle retract.
If you don't need all of the detail, you can simply save the assembly as a part (using the external faces only option) and get something that is pretty gentle on the CPU.
Message was edited by: Gerald Davis on 01/07/10 to update the model - fixed P/N BOM display of rivets; add swage ring on pull handle; corrected over travel on pull handle path.
Here's an assembly in SW09 of a hand held lever operated punch - sort of like a Whitney #7. Handy for making holes in sheet metal.
I've used it in presentations at user group meetings and SolidWorks World for animation studies. The punch and die parts have configurations for standard sizes in inches.
This one isn't really hand tooling, but it is tooling nonetheless. I'll be using this model during my presentation at SolidWorks World.
The cuteness is that you can open the assembly and drag the upper tool towards the die and see the sheet metal "bend" in real time.
The models for the brake tooling have configurations that are based on Amada tooling catalogs.
You might create a test assembly that includes your sheet metal part and the gooseneck tool - position the tool as if it had completed the bend and note any interference between the tooling and your sheet metal part. This is a way to verify that your part can be manufactured with standard tooling on a press brake.
During a presentation at SolidWorks World 2010, Franks and Kidder reminded me of new functionality in SW2010 that makes "legends" easier. The attached 3/8" drive shallow socket is similar to the first 3/8" drive deep well socket example in this thread.
However, the legends are done by configuring the value of the text that appears in the property that is linked to by the sketch that forms the wrap deboss that is the "legend".
That's much easier to set up than the 17 or so "wrap" features that are un/suppressed in each configuration in the deep well model.
Wow, Gerald, it looks like you spend lot of time modeling tools. I don't know how you made the time for modeling all of the tools. It's great that all the sizes are configurations instead of separate models. If I had the time, I would have created some myself. Hopefully I can contribute something one day.
..it looks like you spend lot of time modeling tools...
I used to do drugs but now I model simple things to keep from going completely nuts. Sort of like knitting while waiting for the jury to reconvene.
Time wise, most of these didn't take much more than 30 minutes each. The grease gun was the biggest project, but it will be the theme for my next tour of presentations at user groups.
I sincerely hope you contribute models. A set of phillips head screwdrivers that comport with ANSI/ASME B107.12-1997 would be nice. Hammers, crescent wrenches, crowbar, wire cutters, soldering iron, vice, duct tape, etc. (in metric sizes, of course).
A few of the folks who attended my presentation at SWW2010 requested a copy of the animation that I used to explain why a sheet of sheet metal is thicker in the middle and thinner at its edges. Here's the assembly in 2009 format. There is a motion study that you can use to make your own movie.
I've misplaced the model that I used to explain coil set. Gee, I wish I had a better way to search through my backup drives!
Here is a 3/8" drive ratchet wrench (I think that's pronounced "raht shay" in French).
I recently wrote a magazine column that included advice to leave room for tooling access. Tony H. noticed that I had left room for the socket, but not the ratchet. Everybody is a critic.
So, I made this model to prove to him he was wrong. He was right.
Well here is a set of 3/8" Lettering punches that I use to stamp serial numbers in our trailers. I use the combine function with them because it works better then the form tool. But each punch does have the form tools set up if you want to use them that way.
Gerald, do you happen to have any models of pliers, wire cutters, needle nose pliers. I am looking for a way to make shadow boards for a 5S project. Or do you have any suggestions. I am a beginer at Solidworks.
Here's a model that is based on a set of calipers that were manufactured in 1940 by Moore & Wright of Sheffield England.
Their quick-adjust collet nut is clever and not very well modeled by me - the parts are all there but the method of construction is only implied.
In the real deal 1/2 of the collet seems to be solidly swaged to the knurled nut; the other half floats and is trapped loosely in place by swaging. This lets the leaves spread during coarse adjust and to engage on the screw thread when the collet ring engages. It might be that both of the leaves were supposed to swing and the old dog I have is just stuck. It still works splendidly after 70+ years.
The knurl was modeled using a wrap / circular pattern / mirror. Edit the model and increase the circ pattern to get slightly more realistic knurl - 56 is cute but slow to rebuild.
The screw thread is also CPU intensive @ 4x0.7mm helical cut - my design goal was good looking bling.
Dimensionally and appearance wise this is pretty close. It is missing a few stains and scratches...
The attached step file will make all of the parts without the appearances. The SW14 sldasm has the screw mate and symmetry mate so the legs swing nicely. The spring is not animiated but could be by driving the spring spread dimension with the position of the legs.
(The zipped sldasm holds virtual sldprts for all of the components)
The motion study was created using the explode whiz as a start and then adding fades, camera position
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I really liked using the Style-Spline sketch tool for creating 3D swoop paths. The boundary surface was nifty for modeling the blade cover. This version of the handles is based on loft technology. I hope to demonstrate boundary surface modeling in the follow up model; this version is very sensitive to small changes in sketched profiles. Among other issues with Version 1.0: The end-caps on the handles are not Lombard-quality (yes, Matt we miss you) and the assembly of the swing handle is not shown accurately - it has to rotate 90° before lift-off. Yes, the reference plane used for floor shadows is off a bit, too.
As fair warning, I plan on writing a magazine column about this. If you help me I will take advantage of that help and thank you and acknowledge your contribution but that's it.
I need help with demonstrating best practices in SW modeling of such components. I think my model of the blade cover is okay. The thumb handle is mostly okay - that's what will get a Lombard end-cap in the November column. The finger handle model is a brute force struggle and there must be a better way!
It might be fun to discuss the merits of multi-body models (see the wing nut) vs. assemblies (see finger handle and ball pin). When it comes to manufacturing, BOM and piece-part drawings are a big deal - how does multi-body work for you?
Also, I need suggestions with how to correct the animation of the handle lift-off. I like the work-flow of creating explode view steps in the "correct" sequence and then using the wizard to explode/collapse. In this case, I need to override the explode step of the swing handle. Rather than deleting the explode and replacing it with a distance and angle mate, I'm wondering if there is a way to control when the rotation in the auto-created explode step occurs? Or what other trick would you suggest?
I'll share one.....Attached is a model of the AS568A o-ring with all the dash numbers as configurations with the correct sizes and tolerances using a design table. Enjoy!!
