Transforming toolpaths

[Mick]

Wow, I'm surprised this hasn't already been shovelled into Off Topic with all the political, religious and gun discussions.

 

Should be any moment now. I mean, the mere mention of other CAM systems normally results in a shove off to never never land

 

Hopefully this doesn't get removed, I genuinely just want to see this type of capability added to MC:

 

 

 

 

^ This goes even further and makes it easy to run different parts on different planes and organize your tools in a very efficient way.

 

This type of work and programming is only gaining popularity, we are all trying to make parts for lower price points and this is one of the best ways to do it. If we can reduce programming time it would really help being competitive.

 

What I am wondering is if its possible to add this much capacity into a C hook? I would be interested into putting some money and time into helping getting something like this into MC.

[Sticky]

Wow, I'm surprised this hasn't already been shovelled into Off Topic with all the political, religious and gun discussions.

 

Should be any moment now. I mean, the mere mention of other CAM systems normally results in a shove off to never never land

 

I'm not trying to mention any other cam systems. I am asking how do we get this functionality into Mastercam? Is it possible to make a C hook to do this? Is there some other way?

What would it cost to have a C hook made with this functionality? I don't want to switch away from MC, so I'd be happy to pay to have or help develop this.

[Mick]

It is certainly a nice function. I don't know much about chooks, but I would suspect it is something that could be done.

[crazy^millman]

Well I would say maybe it is possible, but looking at $50K in cost maybe upwards of $250K so have someone develop it. If I knew anything about computer language I would tackle it in a heartbeat. Looking at what Verisurf and Mold Plus do with Mastercam's GUI now I would think it is possible. Build it like their apps where you dock into a tab for the operations manager and go from there. I can do a lot with transform, but have to say nothing like that. Problem is the guy who keeps trying to take food off my and other peoples table for using Mastercam is probably got this already posted up. We all want our job to be easier and this functionality would be a huge step i nthe right direction for those people doing that type of work. NX also has a very nice method for doing this.

[Sticky]

I think its something MC should be considering, the movement for more efficient machining practices increases daily. More and more people are making the switch to hmc's, and those using verticals are using tombstone style fixtures in their vmc's more often.

 

I know right now I am spending lots more time programming compared to my competition, and its not just because I'm slow

[Joe788]

I think a Chook could be made that would do a great job of transforming and rotating toolpaths for a tombstone automagically. It wouldn't be as pretty and feature rich as the Gibbs add-on (I'm assuming that's what Ron was talking about creating), but it would definitely be pretty valuable. I'm pretty sure all the stuff is available inside Mastercam to make it happen for somebody who knows how to do it.

[savagkd]

How about posting each tool group as an incremental sub program, then use a point toolpath followed by a manual entry calling the subs?

[Thee Rickster ™]

It would be nice if CNC would add a tranform option to "transform by point pattern". Cimatron had this capability and it was priceless. Ive made this feature request in the past for just this reason but it never seemed to grow legs.

 

Unfortunately, I have never found a very efficient solution.

 

Send it, again, to CNC so they can try to get it in for X8, ASAP

other wise it may not get into the functionality of MC for years to come

[Sticky]

It would be nice if CNC would add a tranform option to "transform by point pattern". Cimatron had this capability and it was priceless. Ive made this feature request in the past for just this reason but it never seemed to grow legs.

 

Unfortunately, I have never found a very efficient solution.

 

How exactly does this work? I'm trying to picture it but I don't think I'm following you.

 

 

 

 

I think for a simple C hook all we would really need is:

 

-Transform/Translate across a plane/face of a tombstone, multiple instances, with or without specifying pattern shift

 

-"dynamic" type transform/translate where you can pick similar, uneven spaced geometry of the same feature on the same part without needing to set a new workoffset

 

-Transform/Rotate, multiple planes, multiple instances, with or without specifying pattern shift

 

-Ability to set Transform/Translate and Transform/Rotate at the same time (so that we no longer need to transform transforms anymore)

 

-Organize by tool #, or tool paths, or tool groups.

 

-Set independent work offsets for each transformed part (if it just incrementally increased that would be fine too as long as it works on multiple planes)

 

-Ability to enter the center of rotation, and have the option of the post outputting (or not outputting if you want to run from COR only) the work coordinates with G10 for each part and each plane.

 

Anything else?

 

 

If we could have all of the above it wouldn't be too bad to bring in multiple different parts into the file and make a nice multiple part program where the tools are shared across the different parts...

[crazy^millman]

Sticky a good outline and how you properly develop an interface. Look at what it needs to do outline the part so the puzzle it needs to cover. Decide how you want to handle the parts of the equation. Build the logic to support those parts of the equation then start working on the GUI to take the information from the user and then apply that functionality to the item you want. Making a road map from that would be a good start. Take 10 power users and then ask them to layout a common process of what you would like to see for functionality. Then take your idea and combine some of the new Transform logic from MT into the equation and you got something doable. Time line no comment results are you knock everything on its head and customers have another useful tool to get their job done.

[Brian Pallas]

I think I have a solution to this problem. 1. Export your base toolpath, check the box for "Export Operations Geometry". 2. Import you toolpath into a new group, check the box for "Import Operations Geometry". Click OK and it wall ask "Import/Add operation tool group also" I clicked OK, then it will say "Select Operation Origin point". Now this point would be your origin in your base path. So before you do the import operation create points to use as the origin for your new features. So if a corner of your first feature is X7.5,Y6. from Origin, you would need a point that far from each corner of your new features. So import, then select each point, hit escape when you are done. You will get a message saying # of operations imported successfully. Red X out of the Import dialog box. Now you have a bunch of toolpaths in a group. Select all the toolpaths, go to Sort. Under Sorting Options, tool, then by type. Click the box to the right, and arrange the tools in the order you want them used. Click OK. Now your tools should be in the order you want them. Edit Common parameters for all your tool paths and turn "Force Tool Change" Off.

 

That should do what you want it to do. It sounded like all the features were on one part, so I assumed you wanted to use the same work offset. You can get this to work with different offsets, which is what I use it for. Creating a program with 5 parts in it, and getting rid of the tool changes. I have a screenshot of each step in the process, but apparently I am not permitted to upload .bmp files?? Anywho, hope that helps.

[Sticky]

Bob, Ron, Joe etc do you guys have any other input as to what would be useful for a Chook like this? I am going to send a request in to in house to see if they can build a Chook, so I'd appreciate getting other more experienced users opinions.

 

Brian, I am curious to try your method but won't be able to until next week. If you can't upload the screen shots here would you be able to email them to me or someone else here so that they could be uploaded to this thread?

 

Have you used this method to get multiple offsets for different planes/rotations? Specifically using G54 and G55 on B0 and then G56 and G57 on B90 and G58 and G59 on B180 etc. I linked to workaround for this in post #19, but I can't help but think there must be a better way.

[Brian Pallas]

I will email pictures if you want. Can you message your email on this site? Maybe post on here that you sent your email in a message and I will find your message and e-mail.

 

What I do to create multiple offsets, is create the new WCS and/or TCS/WCS planes, assign an offset to that view, and then when you Import your operations there is an option to use the active Planes. Select that box and all imported operations will have that View assigned to them. So you select a view, import, select a view, import..etc.

 

I have not tested it yet with Rotations involved. I am going to see if that works Monday. I have a family of parts we do a couple times a year, and I will put 4-5 fixtures on the table and in the past I have loaded each program into the machine, and then used a program to call the others as subs. This go around I was wanting to eliminate tool changes, and started playing around with this as a method to combine existing programs in an MCAM file.

[Sticky]

I sent you my email in a pm here Brian, thanks!

[Brian Pallas]

I just tried it and this will work with Rotations involved also.

[Sticky]

Here are the pictures that Brian sent me. I haven't had time to try yet, and likely won't for a few more days, but I am really curious to see how it works, particularly with rotations. Thanks Brian!