SW 2000 cut solids 1

[lgbav8r]

Hello everyone,

I am a bit archaic and using SW2000. Anyway, I have made an assembly and joined all parts together and would like to trim excess material from the part. This is a picture of what I am trying to say. I want to trim the "z beams" back to where they intersect each other. Can I do that and if so how? Thanks in advance for the help.

 

[Theophilus]

Certainly. I'd use a Cut With Surface feature to do so.

Perhaps the easiest way to describe this here is to extrude a surface in the exterior Z-beam shape in each direction just like you did with the solid--except you only want the outer edges. (This will be the top, angled, horizontal, and vertical surfaces.) Extrude this set of four line segments each way as a surface (two features--one for each direction).

At this point, hide your solid body so you can see your surfaces. Perform a Trim of the surfaces, selecting the Mutual option--select both surface bodies, and then the two areas you want to keep. You want to keep the surfaces that represent what you want the outer surface of the solid to look like. It should trim to form what you want. Knit the two surfaces into one body (using the Knit feature). Show your solid body again, then select Cut With Surface, select your knitted surface in the feature tree, the direction of the cut (outward) and you should have all that material removed.

I see an I-beam sticking out of your posted image, so you may need to further trim your trimming surface tool either to avoid or include the trimming of the I-beam--depending on what you want.

Kludgey answer and technique, but it should work for you.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[lgbav8r]

Thanks for the quick reply. I will need to trim the I-beam as well but I figured if I can just get one way down I can just copy it on all the rest.

 

[lgbav8r]

Thanks for the quick reply. I will need to trim the I-beam as well but I figured if I can just get one way down I can just copy it on all the rest.

I don't seem to be able to extrude the line segments. Should I be in the Assembly or the part?

 

[SBaugh]

I don't think Cut surface is available in SW00. if it isn't look at using an assembly sketch and turn it into a Cut Assembly feature.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

Depending on how your part is created, you could also edit the extrude features to up to surface.


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[davidinindy]

This is an instance where showing your feature tree would help. It helps us see how you created the part, and therefore, the best way to modify it.

David

 

[Theophilus]

If cut with surface isn't an option, you could nevertheless form the surface and use the surface in a solid cut with the "up to surface" option. I used to do that a lot. You still need to create and knit the surfaces as I mentioned above, and make sure your cutting profile does not bleed out over the extents of your surface or the feature will fail.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[MadMango]

Also, instead of a "cut up to surface", you could also remodel the beams, in-context of the assy, and "extrude up to surface".

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[lgbav8r]

Well I have attached a pic of the file tree for you guys to look at. I did figure out a round about way of solving my problem. I joined all the parts together in the assembly to form a new part. Then I just drew the outlines of the brackets and extruded them out which cut off the edges. I think that's what Theophilus was trying to tell me.

I have encountered another couple problems. First, it does not seem that easy to edit. If I want to take something out of the assembly or move it, etc then I have to rejoin the parts and make the extrude drawings again. Also, I need the different components to be different colors. This is simple in the assembly but in there I can't trim the edges.

 

[EngJW]

You could make a plane near the edge of the beam and draw a rectangle on it, then cut-extrude it up to the surface of the other beam. The rectangle can be larger than the beam cross section or you can make it colinear. Looking at your picture, you might have to do this in two steps so you don't cut away the lower flange of the other beam.

I think this method has already been suggested by someone else, so he gets the credit.

 

[lgbav8r]

Thanks again for the help. Can anyone offer suggestions on coloring the part? I'm not sure separate colors can be used on part files like in assemblies.

 

[MadMango]

Don't color individual faces or features.
Don't color the parts in the Assy file.
Do change the color of the whole part in the Part file.

Tools>Options>Document Properties>Colors

Selec Shading, and then select your color. You can also select Wireframe/HLR and change your color for the times you are looking at the wireframe of the model and want different parts to stand out.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[lgbav8r]

Wow thanks for the help MadMango. I don't think I would have thought about going back to the original part files.

 

[lgbav8r]

Ok. I am getting frustrated. The parts come into the assembly the correct color per MadMango's suggestion. Now when I join everything, it seems all the color properties of the original parts are removed. This is incredibly frustrating as all I want is a simple colored picture. I can't just leave the assembly alone once I import the part because I have to join everything to trim pieces off. Is there anymore advice anyone can give?

 

[lgbav8r]

I haven't figured out how to edit my posts on this forum but I would like to say I think I figured out all of my problems. Basically the whole thing was my stupidity. Thanks to all for your help. It is much appreciated.

 

[CorBlimeyLimey]

For future reference, can you fill us in on what the solution was?
Also, what do you mean by "when I join everything"?

Basically the whole thing was my stupidity

Stupidity & incorrectly using SolidWorks are two very different things ... don't be so hard on yourself.
It's better to ask a "stupid" question, than to make a stupid mistake!


Making the best use of this Forum. faq559-716
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