Mastercam 2022 to Vericut 9.2 (Lathe)

[Simtech]

Hi to all,

Well it's been a while since posting on here, hoping to get some insight on how you guys do things.

I'm in the process of setting up Vericut for toolpath simulation on our mills and lathes, and would like to know your best practices on the lathe side of things.

More specifically, I'm trying to use the MCAMV export to Vericut function for the lathe when using 3D tools setup in Mastercam. The lathe turret setup needs to be adjusted to the gage point of the tool so that everything lines up on the machine. My tools are used on VDI and BOT style turrets on different machines so I want to have the tools transfered from Mcam to VC instead of defining each tool in each machine independantly inside of Vericut.

Also looking into using the "Machining Cloud" for tool definitions inside of Mastercam - curiously, the 3D tools from Machining Cloud exported to VC and the 3D Tools from Mastercam do not match when looking at gage point position. Am I missing something here? For each machine I will be modeling the tool locators (Axial/Radial Heads, Boring Bar holders, etc ...) but would like to have a common database for the standard tools.

Any help would be appreciated.

Thanks!

 

[crazy^millman]

There is a bug in the Interface with 3D tools. The latest interface does a better job at this, but the inserts are still messed up. What I was taught by a very knowledge Vericut person (Thank you Brad Brannan) was to make Vericut inserts to replace the Mastercam inserts brought into the Software through the Interface. Now the software will run a lot faster using the Vericut insert verse the model for the turning operations. I have seen as much as 90% reduction in Vericut times on larger projects using that process.

On the Holders for the Lathe I would make the Blocks and holders for each Turret laid out like you will need. You can disable holder blocks on the turret, but have as many for each position as you want defined. Then as you build you machine you can decided which ones you want activated and then go from there.

With Chucks and Collets chucks I have both built in my Lathes to us then I am swapping them out as needed. I use the same process of Disabling what I am not using and then using what I need for the machine. The Zero Point is easy to control when understood how to realted it to your WCS in Mastercam. CG Tech teaches From and To CSYS to everyone as a way to go about the process. I think that was is terrible and make sure my Zero point is my attach point in my Mastercam file and then never have any problems using the interface to have everything fall right in place in the VMC.

Don't buy into the thought you have to program your part complete before using Vericut. I will build some test operations and then run the interface. You can then make a dummy folder to dump tools and other things into to then import back into the originally created Vericut session without having to redo it everything you make changes or want to add tools to a file.

I also like to take my fixture competents and save them out as one STL verse picking a group of them it can become a rail pain.

Make sure you model tolerance is 1/1 to 1/2 of your finish requirements. If you are trying to hold .001 then make sure the interface is using .0005 for the model export. The default is .004 and seen time and time again reports of false gouges when it was the tolerance being wrong on the model. I also will bring the Step file directly into Vericut and remove the reference turning them into .ply files. Vericut does better with them than .stl and will run faster sometimes.  

[Greg Williams]

Also 9.2.2 has an issue with Ghosted ops. The 9.2.1 Chooks works better

[Simtech]

Thanks for the reply - in the process of setting this up to be used in a school with 3rd year mechanical enginnering students at college level so it has to be pretty straight forward. 

I've been playing around with the MCAMV function for the milling machines (3 axis VMC, 4 axes pallet changer and 5 axis VF3 with TR160) and it works pretty well for now. Tool transfer and part positionning is less of a problem.

Would like to streamline the lathe machines (2 axes XZ, 3 axis XZC and a new Doosan LSYA with sub-spindle). 

Struggling on simple things in Vericut without training (how to stop simulation at each toolchange or at a M01), but getting buy so far.

Again - thanks for the input!

[crazy^millman]

2 hours ago, Simtech said:

Thanks for the reply - in the process of setting this up to be used in a school with 3rd year mechanical enginnering students at college level so it has to be pretty straight forward. 

I've been playing around with the MCAMV function for the milling machines (3 axis VMC, 4 axes pallet changer and 5 axis VF3 with TR160) and it works pretty well for now. Tool transfer and part positionning is less of a problem.

Would like to streamline the lathe machines (2 axes XZ, 3 axis XZC and a new Doosan LSYA with sub-spindle). 

Struggling on simple things in Vericut without training (how to stop simulation at each toolchange or at a M01), but getting buy so far.

Again - thanks for the input!

Right Click on the play button and pick what are your stop conditions and done. You can also click on the space between the block numbers in the NC Program section to create specific break/stop points.

I keep Project Tree/Auto-Diff/NC Program in one window Far Right Screen then keep Vericut Logger and Status in another window. 

Starting this year any customer on maintenance can send one person per license for free training or do online training for free. I am pretty much self taught on the software, but have taken a Machine/Control builder class.

[Simtech]

Thanks Ron - using a new software is like having someone ask me how to show the axis lines in Mastercam (F9). Simple things seem to get it the way.

Would you mind sharing your screen layout? Also, in a classroom context, what would be the easiest way to validate a program from Mcam to VC? Using the MCAMV I would suspect but for the lathe tooling we would need to get into the activating/disabling components in the turret manually.

On the Doosan machine, we are gradually getting up to speed with the Mill-Turn module from Mastercam - do you think the MCAMV will play well between these environements? Haven't tried it out yet.

Will attend the upcoming VUE meeting mid-May and try to get info on free on-line training.

Anyway, thanks for the info - always good to have a Mcam/VC expert on hand to answer questions. Can also serve for others in the group.

[crazy^millman]

2 hours ago, Simtech said:

Thanks Ron - using a new software is like having someone ask me how to show the axis lines in Mastercam (F9). Simple things seem to get it the way.

Would you mind sharing your screen layout? Also, in a classroom context, what would be the easiest way to validate a program from Mcam to VC? Using the MCAMV I would suspect but for the lathe tooling we would need to get into the activating/disabling components in the turret manually.

On the Doosan machine, we are gradually getting up to speed with the Mill-Turn module from Mastercam - do you think the MCAMV will play well between these environements? Haven't tried it out yet.

Will attend the upcoming VUE meeting mid-May and try to get info on free on-line training.

Anyway, thanks for the info - always good to have a Mcam/VC expert on hand to answer questions. Can also serve for others in the group.

Yes learning is part of our job and just had this conversation with a Customer this week. I am always learning and growing my craft.