New to Solidworks

Hi my name is Joe and I just finished the "Parts & Assemblies" course. I've been useing AutoCAD for many years and am trying to get used to working with Solidworks. I design steel racks using steel tube, sheet metal, flat stock, and angle iron etc. Similar to the racks shown on this web site.

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So far I have reproduced a couple of my designs in Soldworks by using my AutoCAD drawings and then making each individual part (tube usually) and then putting them together in an assembly. I understand that using design tables etc you can make one part do the work of many parts. Kind of like if it were wood and you were building a house you could use a rectangular sketch to be a 2 x 4 or a 2 x 6 or even a 1/2" x 48" sheet of plywood x what ever length. So now you have one part with lots of different configurations taht you use to build your house model..... Question is what is the best way to model stuff like I do.... Make each part individually? and put them together? Many times it is just steel stock cut to length, other times it may have holes drilled angle cut ends or be notched and bent (in the case of flat stock and sheet metal)..... Should I use design tables at least for the parts that are just cut to length...... Make a table up for 2" square 12 gauge tube in 1/16 inch increnments up to about 96" long ..... and then 11 gauge and 7 gauge and well you get the idea...... Do any of you guys use Solidworks to design similar products and could you offer any advice as to which is the preffered way I should be headed... I would like to eventually get where I can generate all of the drawings and BOM's etc using just Solidworks... that could be a ways off at the rate I'm giong but I'll keep pluging away... Thanks....

Joe (stuck in A-cad) M reply to : spamplanet at charter dot net

Reply to
Mark Tyme
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We do similar work here and the best that I have settled on is to have a template part, made with a design table, for each raw material, such as angle, channel, beams, etc., each config being an inch long for simplicity. Then when you need one of those materials, you start a new part from the proper template. At that point you have a part file with lots of configs. Choose the correct one for the particular part and create a derived config. Using that config, change the length, etc to suit. If you change your mind on the size of the material, just create another derived config of the new material and switch the assy reference to that one.

The advantage to this system is:

  1. Being able to switch sizes by changing the config.
  2. Having all the materials already set up with appropriate properties.
  3. Once finished (or close) with the design, you can blow away the configs you haven't used, which will be the ones without derived configs.
  4. The design table contains all the info so you can bring them back when you realize you deleted one you needed.


Reply to
Wayne Tiffany


I went to your web site to take a look at the frames. Here are a few suggestions. Do you control your structural members by part number? Example:

12345-12 is 2 in sq x12 x1/16 and 12345-11 is 2 in sq x11x1/16.

Does the part number change for length or when you add holes or angle cuts? Determine how you will name your instances that you can recongize what you are using.

You could have one design table for each major family of part numbers to start. My suggestion is to try to control a few parameters in the design table, test and see if these work in an assembly. Then add a few more parameters and test again.

So as a first run example STOCK contains no other features just length. Example: 12345-12-4FT-STOCK, 12345-12-6FT-STOCK,

12345-12-8FT-STOCK are the instance names in the first column. If the cross section of the structural member is sketched on the Front Plane, the depth of the extrusion will vary from 4FT, 6FT and 8FT. Rename the depth dimension name from D1 to depth. Right-click Properties on the dimension.

Test the lengths.

Add the holes. The state of the Holes (suppressed/unsuppressed) would be in the 3rd column. You could also have column in the design table that control pattern of holes. Rename your features and rename the dimensions you want to control. Think about the dimension scheme so the holes won't fall off into space when the configuration get bigger or smaller. You will have to control your linear hole dimensions. Return to the design table and add holes.

Test the holes.

Add the cuts. If you have different style cuts, then all instances in this column will be suppressed except for the one that you want to show the cut for. Return to the design table and insert the cut parameters.

Test the cuts.

If the design table gets too big to manage create the other size cross sections with a different design table.

Once you get your part design table, you can create an assembly design table based on the instance names of your parts. The first column contains FrameA, FrameB. The second column will contain the instance names of your parts. Spell correctly.

Regards, Marie

Reply to

Thanks for the replies... every little bit helps... We are pretty much a job shop with very little being reused from one project to the next. As far as part numbers are concerned it is pretty straight forward TS2X12-024.50 is 2" square 12 gauge tube

24-1/2" long then if there are holes or any special "features" a six digit job or project number is added to designate that particular part. other examples are TR1.5X2.5X14-110.38 rectangular tube 1-1/2" x 2-1/2" x 110-3/8" long. C04X4.5-036 is 4" "C" channel 4.5 pounds per foot and on and on..

I would like to make it so that any STOCK material where only the length varies could be taken care of with the design tables.. any special parts would be drawn ... oops ... modeled separately... I will try some of the things you suggest as well as what Wayne says works for him which is using 1" long template parts and changing the lengths to suit where it is being used... Thanks for your help, I will continue to monitor this group and will let you know my progress... Joe M

Reply to
Mark Tyme

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