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,
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
RE: Retain tool in boolean remove
RE: Retain tool in boolean remove
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
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
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.
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RE: Retain tool in boolean remove
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
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
RE: Retain tool in boolean remove
We do use a second CATPart for the machining operations.
RE: Retain tool in boolean remove
RE: Retain tool in boolean remove
RE: Retain tool in boolean remove
RE: Retain tool in boolean remove
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
Regards,
Derek
RE: Retain tool in boolean remove
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
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
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
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
Regards,
Derek
RE: Retain tool in boolean remove
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
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
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
You are on the right track, you will only need 1 master file.
Regards,
Derek
RE: Retain tool in boolean remove
Thanks for all your help, I think you have put me on the right path.
thixoguy