Equation Help
Equation Help
(OP)
Anyone know of a good tutorial out there that really explains or shows how to make equasions? If I bang my head against the desk any longer I'm going to need a transfusion. Basicly I have a part with 2 parallel faces offset a distance of 1.44". If I move one face (extrude cut) I need the other to follow.
SBBS....Sorry For Being Stupid.
Bloodclot
SBBS....Sorry For Being Stupid.
Bloodclot
***** Fear not those who argue but those who dodge *****
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RE: Equation Help
... you should be able to use the Offset from surface option when creating the "extrude cut" so that one face is offset 1.44" from the variable face.
... or just dimension the "cut extrude" sketch accordingly.
RE: Equation Help
I have created this extrusion from the midplane using the Ext-Boss/Base. Is it easily done to shorten the part by taking material from the middle? If so, I could form the ends as they need to be and make my shorter configurations by "shrinking" the part lengthwise without touching the ends. Hope that was clear??
h
Bloodclot
***** Fear not those who argue but those who dodge *****
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RE: Equation Help
I know the "established" way of doing things is hard to get changed, but many of your difficulties in modeling these parts will be eliminated if you can follow the suggestions made in your previous thread about "nesting assemblies" and do all your part modelling in the part file rather than adding cut features to an assembly.
RE: Equation Help
h
Thanks
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RE: Equation Help
RE: Equation Help
http:
***** Fear not those who argue but those who dodge *****
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RE: Equation Help
However, even with intermediate drawings there is still no need to add features at the assembly level.
In the case of the part and BOM structure you've shown, I would:
1. Model the "Extrusion" as a base configuration
2. Add a part configuration for the "Cut" and model the cut
3. Add a part configuration for "Machined" and model the machining.
You now have one part file with three configurations. The "Extrusion" configuration has all features related to cutting and machining suppressed. The "Cut" configuration has all features related to the machining process suppressed. Now:
4. Add the part to a new assembly. Make sure the referenced config. for the part is "Cut"
5. Add a configuration to the assembly and call it "Machined".
6. Change the "Machined" configuration of the assembly to reference the "Machined" config. of the part.
You now have one assembly file with two configurations. The "Cut" configuration can be used to generate any drawings needed for the cutting process. The BOM structure will be indented 2 levels as you require. The "Machined" configuration is used in step:
7. Add this assembly to a new assembly. This is the final assembly to make your final drawing. The BOM structure will be indented 3 levels as you require.
Although this does add a couple of steps (adding configurations), it frees you from the constraints of the severely limited number of geometry-modification features available at the assembly level.
RE: Equation Help
Maybe I'm missing something.
Why create the assy's? Why not use the different config's for use on dwgs and within other assy's?
Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)
RE: Equation Help
RE: Equation Help
Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)
RE: Equation Help
BC
***** Fear not those who argue but those who dodge *****
Dell Precision 670
3.0 Ghz Xeon Processor
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Dual 19" Viewsonics
RE: Equation Help
1) Create the cut defining Face 2 as a blind cut using a sketch placed on Face 1. This cut would be along the axis of the tube. This method is the same as handleman’s first suggestion.
2) Create the cut defining Face 2 as a through all cut using a sketch placed on the outside vertical face of the wing that you are chopping off. Dimension the right edge of the cut from Face 1. This cut would be normal to the axis of the tube.
In both of these designs, the position of Face 2 is defined relative to Face 1, and Face 2 should move with Face 1. Simple and no equations involved.
3) Using equations. Start the equation tool while nothing is selected. Click the add button. Then click on the feature for Face 2 and then click on the dimension that you want controlled by the equation. The name for this dimension should now appear in the equation line. Add and = sign after it and then click on features to find the other dimension that you want it tied too. The name of that dimension should then appear in the equation line after the = sign. Then type the rest of the equation / click dimensions to get the result that you want. Depending on how you’ve modeled the part you may only need – 1.44. Then hit the OK buttons on the equation boxes.
4) Using design tables. Since you are doing this for the purpose of creating configurations, you could use a design table that includes the dimensions for the locations of both Face 1 and Face 2 and use equations within the design table to define the dimension for Face 2 based on the value of the dimension for Face 1.
Eric