Transforming toolpaths

[Bob W.]

I have a part with several identical features that involve multiple toolpath operations each and these features are not spaced or located at regular intervals where a standard transform toolpath would be of any use. To program each feature will be very redundant and I was curious if there is a good way to approach this where I only have to program one feature and somehow transform the operations to the other features. My current best guess is to program one feature then do several different transform toolpaths to each other individual feature, but this results in a crapload of tool changes and this is a production part. These features are spaced in the Y direction only but the spacing is random and there are 10 features.

[djstedman]

Not very clean of a solution Mastercam wise.. but maybe program the feature.. make it an incremental Sub-program.. then make yourself a main (written by hand) that calls it from whatever start points you need..

 

You could apply this method to multiple tools as well by simply using the main for each entire tool .. its not really a Mcam solution but sometimes the keyboard ends up being the easiest way to just get it done..

[crazy^millman]

Tool Changes why? Not sure I follow that. You have a .6R to machine and make a contour toolpath for it. Then decide to transform it to 10 places then it gets done in those 10 places. Like of like a parametric program where you have one feature and want it in 10 different places. Assign the concept to one and then go from there. I have a lot of my tombstone programs where I will program the top part then transform down my spacing, then do my bottom operation for the tool and then transform up. Then use copy source operations in Transform and then rotate my rotations for my tombstone and done. It may ve done 16 or 20 or 40 times using only one operation to control that machining on that many parts. I need to make a change I change it on one part and done.

[Sticky]

I have a part with several identical features that involve multiple toolpath operations each and these features are not spaced or located at regular intervals where a standard transform toolpath would be of any use. To program each feature will be very redundant and I was curious if there is a good way to approach this where I only have to program one feature and somehow transform the operations to the other features. My current best guess is to program one feature then do several different transform toolpaths to each other individual feature, but this results in a crapload of tool changes and this is a production part. These features are spaced in the Y direction only but the spacing is random and there are 10 features.

 

Use multiple work offsets.

 

What I do is:

 

1. Program the part as if its just one part all in one tool group.

2. Copy and sort all your different tools/toolpaths into their own tool groups, ie. if you have T1 w/5 paths, T4 w/3paths and T10 w/11 paths I will make 3 tools groups, one called T1 (description of included ops) and include all of its tool paths, another tool group called T4 with all of its paths, and another called T10 and all of its paths all in their own tool group.

3. Now you can create another tool group to transform all of those above groups. If you need to do it on just one plane then use the translate option in your transform op, select how many multiples you want and just leave your XY fields all zeros.

4. If you need to rotate this onto multiple planes I create another tool group to Transform my previous transforms This really turns into a giant pain when you need multiple work offsets...

 

 

I'd love to know a better way...

[BenK]

If I'm understanding you correctly, you will want to place your transform operations after every tool. That way it will run the tool on all the features before tool changing. It will end up with a lot of operations but you will have the result you are after.

[Sticky]

If I'm understanding you correctly, you will want to place your transform operations after every tool. That way it will run the tool on all the features before tool changing. It will end up with a lot of operations but you will have the result you are after.

 

I started doing it that way but then I did a couple jobs with 30-60 tools in them, way too much work trying to find stuff at that point, now even if I have ten tools I still just organize the tools in their own tool group so that its easier to edit both the tool paths and the transform ops when necessary.

[Mick]

I recently had something very similar. A feature and copies of it, but not evenly spaced about the part. The feature required several tools to complete.The procedure was to programme the first operation on the feature, then use transform operations to machine the other features. I then programmed the next operation for the feature, copied the transform operations from the previous op, and reselected the base toolpath. I repeated that until I had all the features completed.

 

It worked perfectly, and with minimal toolchanges

 

That is exactly as BenK describes it above.

[Sticky]

I just realized you are referring to features that are likely staying in the same position from part to part. I kind of assumed this was a part like a casting and the features were in different positions each time.

 

If that is the case then the problem is easier to solve and just requires making multiple transforms from the original path to the locations you need, and you can still use the same work offset.

[kccadcam]

This is how I do it:

Program all ops that need transformed normally.

Transform Toolpath with the settings shown in pics. (set number of instances you need)

Then just assign multiple offsets at whatever locations you need on the machine.

it will run each tool thru all offsets before repeating with the next tool.

 

Is this what your looking for Bob??

[Bob W.]

So with 10 features and 6 tools per feature I will have ten transforms per tool for six tools, for a total of 60 transform toolpath operations, correct? This will run the most efficiently on the machine but will be a bit of a headache to program. Still better than chaining every single feature though.

[Sticky]

So with 10 features and 6 tools per feature I will have ten transforms per tool for six tools, for a total of 60 transform toolpath operations, correct? This will run the most efficiently on the machine but will be a bit of a headache to program. Still better than chaining every single feature though.

 

If you do it the way I was talking about its only 6 transforms, one for each tool/tool group.

 

For example, I just did a program with 32 tools, and most tools had 4-12 different tool paths associated to them. So I created 32 tool groups, and put all the tool paths for each tool in corresponding tool group. Then I just simply create another tool group for transforms only, and in your transform parameters you can just select the entire tool group that belongs to the tool and all the tool paths in it will be transformed, instead of creating a separate transform for each.

 

Sometimes I need to make 2 or 3 tool groups for a tool, just to make it more efficient for certain features, so then I make tool groups named after what type of operation that tool is doing.

 

I don't have a dongle at home so I can't take a screen shot but I could tomorrow when I am back at work.

 

It is time consuming but it does work. I really think MC needs to step on this and work on some better solutions. As soon as you get into what you need to do, and then you need to transform your transform ops to rotate the tool paths with multiple workoffsets it REALLY SUCKS. Unfortunately that is all I do

[NOTW Programmer]

This is how I do it:

Program all ops that need transformed normally.

Transform Toolpath with the settings shown in pics. (set number of instances you need)

Then just assign multiple offsets at whatever locations you need on the machine.

it will run each tool thru all offsets before repeating with the next tool.

 

Is this what your looking for Bob??

I have done this with a max of 4 tools and axis substitution with incremental subprograms. If I remember correctly having the group NCI output option set to operation type, will run the first tool in its entirety before making a tool change. You must have also programmed the T1 and not called it back in a later operation if you only want to see it once. You still have to create separate work offset at the machine for each instance of the features or you can always use G10 and shift the G54 offset for each instance.

 

-Bill

[Bob W.]

This is how I do it:

Program all ops that need transformed normally.

Transform Toolpath with the settings shown in pics. (set number of instances you need)

Then just assign multiple offsets at whatever locations you need on the machine.

it will run each tool thru all offsets before repeating with the next tool.

 

Is this what your looking for Bob??

 

I think that would work except I'm running this on multiple sides of multiple tombstones and with DFO. There is a lot going on there and it would make me a little nervous trying to keep track of it all and keep everything straight. Lots of good ideas in here though. I'll need to wait until the shop quiets down a little (later tonight) to make some sense of it all :-)

[Sticky]

Did you get it figured out Bob?

[Oscar R.]

It is time consuming but it does work. I really think MC needs to step on this and work on some better solutions. As soon as you get into what you need to do, and then you need to transform your transform ops to rotate the tool paths with multiple workoffsets it REALLY SUCKS. Unfortunately that is all I do

 

Hey Sticky, We used to do a lot of transform toolpaths here with the same process that you described above.

We finally got our post guys to modify all of our post to do it without having to create all of those transform operations. Just put the toolpaths in the order that we want and post.

You might benefit from doing the same.

A few hundred buck for a post mod vs. hours and hours of transforming operations is well worth it in my book.

[Oscar R.]

Bob, I had an example MC file all ready to go for you here but it seems that I've reach my file post limit.

[Sticky]

Hey Sticky, We used to do a lot of transform toolpaths here with the same process that you described above.

We finally got our post guys to modify all of our post to do it without having to create all of those transform operations. Just put the toolpaths in the order that we want and post.

You might benefit from doing the same.

A few hundred buck for a post mod vs. hours and hours of transforming operations is well worth it in my book.

 

That sounds awesome! How do you handle multiple workoffsets with the post though?

[Bob W.]

The problem is that all of these features are randomly spaced and each feature uses several tools. What needs to be done is program the first feature to completion, which involves several tools. Then I do one transform toolpath operation to the second feature, then create another transform operation to the third feature, etc... until all ten features are machined. With this method each transform toolpath operation will run through all tools until the feature is complete which involves several tool changes.

 

The method outlined by Kevin C would work but it makes me nervous tracking all of the work offset changes for G54 and G54.1 on multiple tombstone sides and multiple pallets. I can't just create one transform for an operation group because the spacing for each feature varies from one to the next.

 

These features involve surface machining and creative 3D contours so programming each one would be a real headache. Still working on it. I think for now I will just deal with the tool changes to get things running and try to refine from there. Am I missing something?

[Sticky]

The problem is that all of these features are randomly spaced and each feature uses several tools. What needs to be done is program the first feature to completion, which involves several tools. Then I do one transform toolpath operation to the second feature, then create another transform operation to the third feature, etc... until all ten features are machined. With this method each transform toolpath operation will run through all tools until the feature is complete which involves several tool changes.

 

The method outlined by Kevin C would work but it makes me nervous tracking all of the work offset changes for G54 and G54.1 on multiple tombstone sides and multiple pallets. I can't just create one transform for an operation group because the spacing for each feature varies from one to the next.

 

These features involve surface machining and creative 3D contours so programming each one would be a real headache. Still working on it. I think for now I will just deal with the tool changes to get things running and try to refine from there. Am I missing something?

 

Are the features all fixed to a single datum? Can you use a single work offset per part?

 

If they are, then this is what I would do:

 

-Program the complete feature with all tools in its own toolgroup (toolgroup1)

-Make a new tool group for just transforms, and transform everything from the first tool group to all of the unique locations, you mention 10, so you should have ten transforms here.(toolgroup2)

-Now make a tool group for each tool, lets say you have 15 tools for the feature in your first tool group, this means you need to create 15 new tool groups(toolgroups 3-18)

-Now COPY tool group 2 into tool groups 3 through 18

-You can now edit the transform parameters in tool groups 3-18 to use the only the tool number for the correct group from tool group1. The reason I suggest doing it this way is so that your transform XY values will be consistent amongst all 150 transform operations you have up to this point, you only need to rely on repicking the toolpath.

 

If you need to rotate this around a tombstone all you need to do at this point is create another tool group, and create an individual transform for each tool, so another 15 transforms in this case. Hopefully you can use a single workoffset per side. If not there is even more work to be done:

 

http://www.emastercam.com/board/index.php?showtopic=75573

[neurosis]

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.

[Bob W.]

How about the dynamic transform for geometry? I can select several geometric entities then copy the entire set of entities to multiple locations by just pointing and clicking and it goes very quickly. It would be great if there was similar functionality for toolpaths. Drilling and tapping a series of holes comes to mind. Select one hole and program the spot drill, drill, tap, and countersink, then just point and click to the remaining holes and ALL operations for that cycle are transformed. I know holes are pretty simple already with copying geometry etc... but you get the picture.

[Sticky]

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.

[crazy^millman]

Sticky thanks for posting that. Not sure if it will stay or not if it were my board it would not.

[Sticky]

Sticky thanks for posting that. Not sure if it will stay or not if it were my board it would not.

 

I'm not trying to slam Mastercam, I just want to see if there is anything we can do to implement these capabilities into MC.

 

It might be for a small market, but I know there are plenty of people that program 4 axis mills here that could benefit from this. Unfortunately for me I only program hmc's so these types of benefits would pay quickly. If I could buy a tombstone add on for Mastercam that has the same type of functionality for $2500-3kish it would have an ROI of about a couple weeks in my shop.

[crazy^millman]

I'm not trying to slam Mastercam, I just want to see if there is anything we can do to implement these capabilities into MC.

 

It might be for a small market, but I know there are plenty of people that program 4 axis mills here that could benefit from this. Unfortunately for me I only program hmc's so these types of benefits would pay quickly. If I could buy a tombstone add on for Mastercam that has the same type of functionality for $2500-3kish it would have an ROI of about a couple weeks in my shop.

 

I see the benefit and it is a very nice way to do things. Anyone who would argue it does not have merit just has never have to program machines like this.