Retain tool in boolean remove 1

[thixoguy]

Hi All,

I am wondering if there is a way to retain the the solid that I use in a boolean remove other than first making a copy of it? In UG there is the option "retain tool/target".
Anything similar in catia?

Thanks,

 

[jackk]

If we're talking V5: it's still there, even after the boolean operation. (as is every other element/feature you make). The 'solid' (Part Body) is automatically hidden when the operation is added, but you can show it.

 

[thixoguy]

But can I re-use that same solid in another remove operation without making a copy of it?

 

[jackk]

Probably not, unless you do a copy&paste with link. (I'll try it myself on Monday)

I'm having a hard time trying to figure out why you want to do this. Could you provide more details and maybe a picture?

By the way, I agree with you comment about the documention. V4 had much better reference material that I find is very lacking in V5. But V5 is much better with the online training material - it just doesn't explain everything.

 

[thixoguy]

Jackk,

I am designing a mould and what I do is create a master file. In this file I have my part( the part to be moulded)and I create my core and cavity blocks along with my parting surfaces. I then subtract the part to be moulded from the core and also from the cavity and then trim each to my parting surfaces. So I need to subtract the moulded part two times (one time for core,one time for cavity).
I then copy and paste the core and cavity blocks to seperate files and finish off the rest of the mould.

Getting back to my original question I suppose the only way I can use the moulded part twice is to copy/paste.

Thanks for your input Jackk, it is appreciated.

thixoguy

 

[solid7]

Getting back to my original question I suppose the only way I can use the moulded part twice is to copy/paste.

Probably, it is - but you say that like it's a bad thing. (???) In actuality, it accomplishes the goal, and does it very neatly. (allowing you to externally modify the cavity/core geometry, should you need to do so)

Power copies are an option, as is pasting with link.

---
CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[jackk]

I'm working on a casting right now, so I understand what you're trying to do. I also just did a little test to verify how CATIA handles this.

As you probably already know, you cannot do a boolean operation on a solid (partbody) more than once.

So you need to copy the partbody of the part and paste special (paste with link) to create a new partbody with a linked duplicate of the solid. You can then remove the part from the second die block.

The trick to make this work is to use "paste with link," so you'll only have to change the part once and the linked copy will change also.

If I understand your posts; your part is in a separate 'master' CATPart file from the tooling, and your core and cavity blocks are in the same CATPART file. So I guess you are already copy & pasting the 'master' partbody to the second CATPart. Just do a second paste special with link so you'll have two partbodies to be removed.

 

[thixoguy]

Jackk,

Thanks for your help jackk. I have in fact done just what you have explained. I suppose I was initially just looking for some sort of shortcut.

 

[catiajim]

Your best bet here is to make sure that your parts are in different CATPart Documents. One for the casting, and one for each of the mold halves. Then just Copy/Paste Special, As Result With Link the casting into each of the mold halves. Use this for your boolean subtract. This can be done either Contextually (inside of an Assembly) or individually (with the CATPart windows tiled)

 

[jackk]

I have to disagree with you Jim, on this one. We make the casting as a single CATPart. Each die block and any other cores (side pulls) are in partbodies with booleans. This works very well for us for castings and plastic molds.

We do use a second CATPart for the machining operations.

 

[DBezaire]

We build full mold assemblies in contextual mode, definitely the way to go. Previous methods of a single CATPart work, but not as efficient as a Product structure.

 

[jackk]

Derek - are you doing part design or mold design?

 

[DBezaire]

Jack - mainly mold design, some part design.

 

[thixoguy]

Thanks for all the input, people.

DBezaire, I am just wondering where you create all your parting surfaces? Are they in a seperate catpart as well?Also,please explain the advantages of working in the product structure.
Any tips for a catia newbie would be greatly appreciated.

 

[DBezaire]

thixoguy - We create a "master parting line file". the majority of parting line work is done here. in this file you create your core and cavity splits. We build both simple and complicated tools in this manner. Once you set up a default tool template the creation of a full mold in assembly mode is simple. If you have large data sets you can work in cache mode, this allows you to have the entire tool assembly loaded into Catia. If you make updates to your part or parting line, the appropriate files are updated as well. You can load a small sub-assembly up if you want to work on a local change. All items are accounted for automatically in the bill of materials. Data overlays are performed in seconds. The list goes on

Regards,
Derek

 

[jackk]

Thanks Derek. I'm doing part design, but we're very particular and aware of parting lines, shutoffs, gates, etc and their effect on the appearance of our parts.

The more I think about it, Assembly Design does make sense for mold design work. Your molds are probably more complex than some of our final products (but ours are prettier!)

 

[thixoguy]

Derek,
Thanks for all your input, it is greatly appreciated. But I would like to continue picking your brain if I could.

1. How would you handle say, a 4 cavity tool with slides?
Would you create your slides, gibs and wearplates at the assy level or in seperate catfiles and then constrain them in the main assy?

2. Does your final tool design consist of one product(complete mould assy) and individual catparts or do you create several sub-assys?

Thanks again.

 

[DBezaire]

thixoguy - It was a busy weekend, brain may not be worth picking.

1)Every mold component should be an individual CATPart. If the 4 cavity tool is created in 1 solid block opposed to 4 inserts mounted on a common plate, translate and rotate the surface geometry in GSD with Datum on. If you update 1 cavity, the other 3 will follow. 1 slide would need creation in a seperate CATPart - at the assembly level instantiate 3 copies. Same should follow for gibs and wearplates. These items should be created and kept in a catalog of parts.

2) Final design is 1 assembly consisting of many sub-assemblies of individual CATParts.

Do you publish your geometry? Are you keeping the links with selected objects? 2 options in Tools-->Options-->Part Infrastructure-->General.

Regards,
Derek

 

[amitkulk]

Hi....

I will suggest to use the Hybrid Design for this situation. This enables you to create a tool Body and use it multiple times where you need. But if you modify the main body it makes change to all the locations you have used it.

Hope this helps you..
Amit

 

[DBezaire]

You don't need Hybrid design for that, copy/paste special - as specified in Product Structure at the assembly level performs in this manner. I have yet to find a significant advantage to hybrid design.

Regards,
Derek