Equation Help

[bloodclot]

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

***** Fear not those who argue but those who dodge *****

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[CorBlimeyLimey]

Sorry I don't have a tutorial link for you, but instead of using an equation;

... 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.

​

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[bloodclot]

CorBlimeyLimey - I do not have the option of offset from surface. I only have Blind, Through All, & Midplane. This may be because I am in a SLDASM and not an SLDPRT. Is it possible to do an Ext-Cut with a 3D sketch? If so, I could sketch the profile of the 2 faces to each other and then do the Ext-Cut.

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??

http://img381.imageshack.us/img381/3244/endsuv3.jpg

Bloodclot



***** Fear not those who argue but those who dodge *****

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[handleman]

Say your longest part is 8". Start with a base part that is 9" long and cut-extrude 1/2" on each end to create 8" total length. This will create "Face 1" in your drawing. Now cut-extrude again 2" to create "Face 2".

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.

 

[bloodclot]

Adding the features in the assy file is the only way i can do it because it follows the manufacturing process. 1st we extrude then we add this machining process. By adding the machining process we have to make it an assy file. If I was to create a BOM for this assembly it would only consist of an assembly of processes rather that components. I have no choice but to model following the mfg process. Here is a picture of the TREE.

http://img101.imageshack.us/img101/6458/treelj7.jpg

Thanks

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[handleman]

Previously you stated that there are not any intermediate drawings created showing the processes. Therefore, modeling the process in an assembly is of no benefit. If you need the layered assembly solely for the final BOM, model your finished part and then insert it recursively as many layers deep in assemblies as you have processes. There's no need to add features in the assembly.

 

[bloodclot]

In the case of this part it goes like this.

http://img314.imageshack.us/img314/175/bomlayoutnz8.jpg

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[handleman]

I apologize, I may have misunderstood one of your previous posts. I thought you had said that you make no intermediate drawings. Now I gather that you do make some intermediate drawings.

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.

 

[ctopher]

handleman,
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)

 

[handleman]

It's to achieve the indented BOM structure that's required for bloodclot's MRP system. The final drawing has to have a BOM showing all steps.

 

[ctopher]

Oh, Thanks.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[bloodclot]

handleman - OK, I'm going to give your suggestion a try and see how it works. I'll let you know hopefully this afternoon.

BC

***** Fear not those who argue but those who dodge *****

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[EEnd]

I am unsure how you have your part modeled. A picture of the part before and after the cut defining face 2 may help clarify how you have modeled it. Looking at your image I have a couple of possible suggestions on making the geometry behave as desired.

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