Ever wanted to put a Center Mark on an Isometric view in a drawing ?
You can’t do it with the regular “Center Mark” tool, but the video below shows a pretty good solution…
VIDEO — ISO CENTER MARK .mp4
And here is the .sldblk file I created… ISO CENTER MARK .sldblk
This is a follow-up post to a question that I was asked recently about THIS blog entry: http://www.3dvision.com/wordpress/2012/04/14/strengthening-ribs-in-sheetmetal-new-in-sw2012/
The question was basically “HOW do I MAKE a rib like that ?”
Easy !
Start out with this:
Then create your “Rib TOOL” as a separate BODY in the file…
Then you can use the INSERT–FEATURES–INDENT command to use that “Rib Tool” body to create the indentation in the sheet metal part.
You will then of course want to do a DELETE BODY on the Rib Tool body (just select the body in the tree and hit Delete on the keyboard), and then add any fillets (don’t forget both sides) if you want them to make it look something like this when finished.
Here is a link to the actual SolidWorks part file (2013 version) if you need more guidance: Sheetmetal REMOVE FACES
There you go !! Easy when you know how… 
I want to clear something up that is very confusing about making SUB-WELDMENTS.
I personally had swayed people away from the Sub-Weldment functionality for quite a while, because after you went to all the trouble to get all the properties you wanted in your Cut-List Items, you would lose it all when you made a sub-welment,
NO LONGER THE CASE AS OF SW2012 !!
Trust me, it DOES work, BUT it is somewhat confusing HOW to do this the CORRECT way…
The thing to remember with this is that the BODIES do NOT store any properties, only the Cut-List Item FOLDERS do.
So if you have never done an UPDATE to the cut-list first, you cannot expect the properties (that don’t exist yet) to propagate down to the sub-weldments like they are supposed to !
It sounds obvious when I explain it that way, but it was very confusing to me for a while, and I know it is still confusing to new users…
HERE are the steps TO SUCSESSFULLY MAKE A SUB-WELDMENT:
1. Go and create your weldment as normal
2. Update the cut-list
3. Ctrl+Select the BODIES you want to make into a sub-weldment (either from tree or from screen with bodies filter)
4. Rt+Clk, CREATE SUB-WELDMENT
5. Then UPDATE THE CUT-LIST AGAIN !!!
(you will end up with 3 levels in the folder which seems strange, but it DOES inherit the properties into the Sub-Weldment like it is supposed to…)
This will even take the properties with the sub-weldment if you save it out to a separate part file (using rt+clk, insert into new part on the sub-weldment), and they will be tied/related back to the original weldment file for updating !
Hope this helps !
Remember, as an alternative to actual “sub-weldments” done this way you can always just make a weldment, make another weldment, and then stick them into an assembly together. The above method just keeps it ALL in ONE multi-body weldment PART file. And NOW IT WORKS THE WAY IT SHOULD !
To review, I had 4 main design criteria for the Remote Control Hover Craft.
I proceeded forward with the design of the Hovercraft using SolidWorks 3D mechanical design software. SolidWorks allowed me to quickly develop and execute a first pass design, utilizing Multi-Body Parts, In context Assembly Modeling, Sketch Pictures, Fastening Features, Interference Detection, and several other standard options. All of this came together in an initial design that meets the above criteria.
The design started with the Top Plate part that houses the downward facing fan assembly and gives the craft its overall dimensional size. I kept the craft under the 8″ by 8″ tray size of the Stratasys UPrint 3D Printer. The part consists of multi-bodies; one for the plate and the other for the fan housing. These bodies have minimal tolerance so they are a snug fit when pressed together for final assembly. This design criteria is so that if the propeller needs to be serviced later total dis-assembly of the craft does not have to take place. Simply pull the fan unit upward out of the top plate.
Top Plate
Exploded View Front
Exploded View Back
The chassis continues with a bottom plate and separating ribs. The chassis is hollow as the air needs to fill this cavity before exiting out of the skirt. The skirt is intended to be a bicycle inner tube cut to size with holes cut around the inner bottom portion allowing the air to escape. The skirt will be held on by two fastening plates and standard hobby store machine screws.
Section View
The back cowling snaps into place with a Snap Hook. The Fastening Feature command was used to create this geometry. The Snap Hook will allow for ease of assembly, and the cowl contains a cross bar with built in motor mount sized for a 9V-11V brushed can motor. The Cowling and Top Plate will make up the mounting location for the dual rudder system. The system is driven by an S75 Nano servo available at most local hobby shops.
Cowl
The canopy will cover all of the electronics including the Receiver, two Electronic Speed Controls (ESC), And two Li-Poly 300MAH 11.1V Batteries. One ESC and battery per motor. I originally set out utilizing the Sketch Picture and Surfacing to create the canopy structure. This worked out well, however at this time I did not have the electronics in the full assembly. When trying to accommodate the electronics under the first variation of the canopy I visibly had interference. Luckily utilizing in-context editing and having a well planned design intent, the changes to the canopy allowed for an easy and quick change.
Sketch Picture
Interference Original Canopy
Receiver & ESCs
Batteries, Receiver, and ESCs
Canopy Design Change
There is still much to do with the modeling aspect, but for now I have a good working start to the project and a starting point to investigate the flow and stress characteristics of the design. The next step is to utilize Flow Simulation to verify the lift ability of the motor and propeller combination for the lift fan and the rear facing fan assembly.
Top
Front
Back
Side
For this blog series I wanted to design something from scratch. Not necessarily a new idea but something fun and cool. My intention is to design a Remote Control Hovercraft from the ground up.
A hovercraft or air-cushion vehicle is a vehicle capable of travelling over variable surfaces, such as land and water. The hovercraft operates by forcing a high pressure of air between the bottom of the craft and the surface below. This high pressure of air lifts the vehicle upward essentially “hovering” above the ground on a cushion of air. The first practical design for hovercraft derived from several coinciding inventions in the 1950s to 1960s. They are now used throughout the world as specialized vehicles for transport and other applications.
I have specific goals in mind that I want to meet in the design and build of this project.
I am starting from just an idea, and a sketch. We will see where the design leads.
If you attended one of 3DVision’s “What’s New in SolidWorks 2013″ rollouts or even if you were a good user and read the “What’s New” guide for 2013, you hopefully saw something about the new automatic BOUNDING BOX that gets created for plates in Weldments.
But, if you don’t do weldments you may have also thought, “SO WHAT ?!”
Well here is WHAT…
You can use the new automatic bounding box tool for ANY kind of part !!
Say for example you want to find the material needed to machine a part.
Once you get any SolidWorks part modeled (or imported), use the INSERT–WELDMENTS–WELDMENT feature to “turn it into a weldment” (even though it really isn’t), then Rt+Clk the “Cut list” item in the Feature Tree and choose UPDATE. Expand the “Cut list” item in the tree, Rt+Clk the “Cut-List-Item1″ folder that got created, and choose CREATE BOUNDING BOX.
If you just want to see the 3D bounding box that got created, expand the “Cut-List-Item1″ folder and SHOW the 3D Sketch that was created. If you don’t like how the bounding box is oriented, no problem. Just another Rt+Clk on the “Cut-List-Item1″ folder and choose EDIT BOUNDING BOX !
You could add reference dimensions to the bounding box if you wanted to actually show some dimensions, OR if you just want to know what the dimensions of the box are, guess what you Rt+Clk on ??
Yep, the “Cut-List-Item1″ folder once more, and this time choose PROPERTIES.
In here you will see the Thickness, Length, Width, and Volume of the 3D Bounding Box !
AND of course, if you make ANY changes to the size of the part file, the bounding box updates !
Pretty great new feature in SolidWorks 2013 that can save you a lot of time and definitely NOT just for Weldments !!
You are personally invited to join 3DVision and the SolidWorks Technical Team for a new monthly webcast series, “Coffee with the CAD Guys”. This series of educational webinars will be held monthly and will last 30 minutes each.
The first new webinar to be offered this month will be: Going 3D by leveraging 2D.
With all of the 2D drawings you have I bet you wondered if they would be any good if you were to move to 3D. Well your 2D drawings have value and we’ll show you. By using DraftSight to open and edit your 2D drawings you can also use it to help create 3D solid models. That’s right, going 3D by leveraging your 2D drawings.
This webinar will be offered:
Friday, February 15th from 8:30am – 9:00am Eastern Time.
To register for Going 3D by leveraging 2D click here.
The second new webinar to be offered this month will be: Overview of SolidWorks Electrical.
More and more products have embedded electrical content, including power systems, user controls, complex wiring, and harnesses. SolidWorks Electrical simplifies electrical system design with its intelligent design tools, comprehensive parts database, and real-time integration of your 2D schematics and 3D models.
This webinar will be offered:
Friday, February 15th from 9:30am – 10:00am Eastern Time.
To register for Overview of SolidWorks Electrical click here.
So join of us for one of the above webinars on February 15th, we look forward to you joining us.
Ever wanted to look at the same part from different views ?
Well there are two nice ways to accomplish this in SolidWorks…
One way is to use the WINDOW–VIEWPORT–TWO VIEW or FOUR VIEW commands.
You will then be able to rotate one of the views to look at the Front of your part/assy and another one to look at the back, etc.
The second way is to use the WINDOW–NEW WINDOW command.
This will “clone” the window you have active but you don’t really see it.
So then you do a WINDOW–TILE VERTICALLY or TILE HORIZONTALLY to see the two windows looking at the same part/assy.
This method is also great for looking at two different sheets of a DRAWING at the same time ! Where as the first method won’t allow this in a Drawing.
Want just a little more guidance of “where” you are at in a Drawing in SolidWorks ?
TURN ON THE RULERS !!
Most people have no idea about this option, so don’t be embarrassed. :-)
Just go up to the VIEW pulldown menu, and towards the very bottom turn on RULERS !
Don’t forget you also have the cursor coordinate numbers at the bottom of the screen… The rulers are just easier toquickly look at and understand where you are on the sheet, especially if you are zoomed in.
This is great for when you are sketching on a drawing or using snapping with the grid on a drawing.
Don’t forget, SolidWorks 2013 is not going to run on Windows XP. This includes SolidWorks Enterprise PDM 2013 viewers too. I know many of you have older shop floor computers working as vault viewers…so remember to get some upgrade money in your budget.
Looking into my magic crystal ball, 2013 may be the last release for Vista…and Windows Server 2003.
Good riddance to Vista, but this could be big news to those of you that have EPDM running on Windows Server 2003.
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