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Retain tool in boolean remove

Retain tool in boolean remove

Retain tool in boolean remove

(OP)
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,

RE: Retain tool in boolean remove

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.

RE: Retain tool in boolean remove

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

RE: Retain tool in boolean remove

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.

RE: Retain tool in boolean remove

(OP)
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

RE: Retain tool in boolean remove


Quote (thixoguy):


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.

RE: Retain tool in boolean remove

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.  

RE: Retain tool in boolean remove

(OP)
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.

RE: Retain tool in boolean remove

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)

RE: Retain tool in boolean remove

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.

RE: Retain tool in boolean remove

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.

RE: Retain tool in boolean remove

Derek - are you doing part design or mold design?


RE: Retain tool in boolean remove

Jack - mainly mold design, some part design.

RE: Retain tool in boolean remove

(OP)
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.

RE: Retain tool in boolean remove

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


RE: Retain tool in boolean remove

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!)

RE: Retain tool in boolean remove

(OP)
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.

RE: Retain tool in boolean remove

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

RE: Retain tool in boolean remove

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

RE: Retain tool in boolean remove

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

RE: Retain tool in boolean remove

(OP)
A great big thanks to all, especially Derek!! Have a star!!
But I am afraid I have yet, some more brain picking to do
(I really should fedex you some tylenol)

Getting back to the 4 cavity tool, how would you handle it if ,say,the parts needed to be in seperate inserts with each cavity having a slightly different cooling configuration? The way I would do it is bring in my master file 4 times and constrain it in the mould assy. I would then create a new file for each  core and cavity insert (4 cavity and 4 core in context of the assy) and then I would copy/paste with link  a "master core or cavity" into the respective new files. I could then create seperate water configurations for each insert yet maintain associativity if any engineering changes come up. Is this how you would approach it?


I don't publish my geometry( I will try to read up on that)

I also keep links with selected objects.

Also, do you use the mould design package? We have it at my new job but I would prefer to  design without it for now until I get a little more experience in Catia.


Thanks again ,thixoguy

RE: Retain tool in boolean remove

Thixoguy -- if I could only take the star and put it on my refridgerator!  Thanks.
Publications are a time/date stamped pointer that will provide stability to your assemblies.  Nothing much to do other than publicate the geometry that you want to share and toggle the option I metioned earlier.
On to the 4 cavity.  I need a bit more info from you
1) how large in MB is the part file
2) could your workstation handle 4 cavity inserts in at once
3) if you are not using publications you must be working in design mode and not visual.  Difference being cache turned on in options.
4) Using CATDrawings with this?
5) Attaching water fittings as CATParts

Regards,
Derek

RE: Retain tool in boolean remove

(OP)
DBezaire,

 I am not actually creating a 4 cavity tool at htis time, so I don't know how large the file will be but I am pretty sure my work computer can handle 4 cavities at once. What I am more interested in is the actual procedure involved. Is it like the way I described it in my earlier post?

I am going to start using publications, they seem quite useful.

I will be creating drawings for all components.

Fittings,screws,corepins and ejector pins will be seperate catparts.

Thanks again, thixoguy

RE: Retain tool in boolean remove

Thixoguy - I am going to assume it is 4 cavity inserts on 1 common plate.  If this is true you have a Master parting line file containing 1 join of cavity data with split lines large enough to split the insert block (reason I keep assuming 4 inserted blocks on 1 common plate - you stated seperate different water circuits for cavity).  Pitch and rotate the remaining 3 cavities for later use.  Publish out the cavities.    In your assembly you should have 4 separate CATParts (for each insert)  Make 1 of these CATParts your lead cavity insert.  I would build the insert around ABS zero. Also build all the common items in 1 chunck of the solid structure.  After this you can Assemble the features.  This will create a new body under an assemble command. Publish this new body out for the remaining 3 cavity blocks.  Copy/paste with link to the other 3 cavities.  The subtraction for the water circuit should appear after the assembly command in the master Part body.
You are on the right track, you will only need 1 master file.

Regards,
Derek

RE: Retain tool in boolean remove

(OP)
Derek,

 Thanks for all your help, I think you have put me on the right path.

thixoguy

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