How to create a negative from a holed solid block?

[engmechs]

Hi guru,
I am going to create a hydraulic control block with many ducting channels/ holes inside it.

Want to find an effective way to view/ edit the channels within the block.

Can I first create a block, then create the channel later, & convert the channel from hollow to solid? In other words, create a "negative" out of the channelled block in this case?

Please give me some tips.
Thanks in advance.

 

[cloche]

If I understood well, you can model the block and each of the pipes separately (i.e., as separate solids within the same part: just uncheck "join solids" in the Feature Manager when you create them), then subtract the pipes to the block with a boolean feature (only from SW 2003 - you can't do that with earlier versions).
By this way, if you want to roll-back to the "separated state", just suspend the "subtract" feature.

Claudio

 

[SBaugh]

I think "cloche" is talking about the Combine tool that allows you to Subtract, Add or Combine separate bodies from or too other bodies within a single part.

See help on "Combine" tool

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[cloche]

Exactly.
Sorry for the approximate terms I used, but my interface is in Italian and I don't switch it often to English...
"Combine" is also able to discriminate for separate solids that are ingenerated by the operation itself. For ex., if you subtract a pipe to a cube, there will be two solids as a result: the "drilled" cube and the "water inside" the pipe. SW will prompt you if you want to keep both solids, or select which to keep.

Claudio

 

[Theophilus]

In SW 2005, you can also use the Indent feature--something new. The interface on this new feature is still a tad difficult to understand, but it works well (I just found a good use for it in punching indents for strength into a sheet metal part last week).

I think you could adapt this feature to your uses as well as the solutions above.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[engmechs]

Thank you A LOT for you guys help!

 

[MElam]

You could also do this with a "Cavity" (insert new part first). Check it out in the help file.

 

[aamoroso]

I was thinking the same as MElam, put your contraption into a big block and cavity it, the pipes will be solid inside the block so you may have to cut the block down to get them out of it but they will be exactly what you need.

Fill what's empty. Empty what's full. And scratch where it itches.

 

[EngJW]

Just did something similar with a cylinder head. I designed the combustion chamber, intake port, and exhuast port as separate parts so that I could get at them easily. Then I started a new part and inserted these parts into it. It was a little awkward trying to get them into the right positions as you don't have mating operations like in an assembly. Eventually I did a combine for the whole part. I found that I could go back to the original parts and make a change but it was not automatically picked up without doing some other operations. I'm not sure what the right way is but it was something to do with viewing the external references.

I don't know if I would do it the same way next time. I didn't think of making all the components in one part file.

 

[SBaugh]

That's why if you made to separate bodies in one part you can subtract those bodies and you are left with the part you want. It's much easier to do then it is to explain it I think.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[engmechs]

Hi jlwoodward,
When you create one part with relationship based on the other one, it will have assoications/ links with them. Beware that when external reference link exists, it is very easy to change the parts without notice. I normally broke the links between them.

Thanks again for all replies. Very cool.

Edward

 

[CorBlimeyLimey]

An alternative to the Combine feature:-
1) Create the block.
2) Create a Swept-cut for the channels.
3) Create a Swept-boss using the same profile & path as the Swept-cut, but deselect the Merge results option.
4) In the Solid bodies section, hide the Swept boss body.

The advantage of this method is that you can directly get the mass properties (volume) of the Swept-boss body (whether hidden or showing).

Using the Combine method, you have to suppress the Combine feature before being able to get the mass properties & then have to unsuppress it to return the model to the finished state.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[SBaugh]

That is what I have been saying all long. Use the Combine/Subtract feature.

Cheers,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[CorBlimeyLimey]

Wow, Scott ... I thought I stayed up too late at 23:12, but you "won" last night (this morning) at 0:18

BTW, I was suggesting an alternative to the Combine/Subtract method.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[SBaugh]

HELLO!!! Wake up Mr. Baugh... your coffee is right next to you!

I need to read a bit better!!

I feel stupid now -

,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[CorBlimeyLimey]

Early night tonight, right ???


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520