Horizontal Programming your method?

[Colin Gilchrist]

Bob,

 

To speed up the Plane creation, here is what I recommend. Create a 'Template' file that has you common planes (0, 90, 180, 270, and any others you commonly use (45 degree increments?)). Save this file in a good location.

 

Now when you start programming a new job, open the View Manager. In the View List, Right-Click and select 'Import'. Now browse to your Template file and Import the Views you need for the new file.

 

Another option is to start by opening your Template file, and then do a Save-As and create a new part file. The problem is that you can easily overwrite your Template file by mistake if you forget to Save-As and use a new name.

 

 

Andante,

 

Both methods are acceptable, and it really depends on personal preference.

 

Here is my take on it, and this is just my opinion, not an "official" endorsement. By Default, CNC Software's Horizontal MD/CD/PST files are setup to use Top WCS and Front Toolplane. Front Toolplane is set to output B0.

 

The advantage to using the Top/Front method of programming has to do with the way our Planes are setup. When using Top/Front, the Front, Right, Back, and Left Planes are constructed with the X+ direction oriented the correct way for each 90 rotation.

 

This means you can use the Front/Right/Back/Left planes in Mastercam, "out of the box", and get the proper B axis rotations output by the Post. Many people combine the Toolplane Indexing with 'Automatic Work Offset' creation. This feature will assign a new work offset (G54, G55, G56, ect.) every time the Post sees a Toolplane change. This will give you G54-B0. for Front, G55-B90. for Right, G56-B180. for Back, and G57-B270. for Left. This is assuming you only used those 4 planes, otherwise the Automatic Work Offset numbering will just output the Work Offset numbers sequentially.

 

Personally, I do not use the 'Automatic' work offset numbering when I'm programming a job. I set a Work Offset number on each Toolplane I'm using, that way I always know what Work Offset value I'm going to get when Posting. (again, just my personal preference).

 

As others have mentioned in this thread: the drawback to using Top/Front for programming a Horizontal is the difficulty in transferring a program from a Vertical machine to a Horizontal machine. If you setup all your Posts for Top/Top style programming, then it is easier to swap programs among your machines.

 

The thing I really like personally about using Top/Front for programming a HMC is the display in Backplot and Verify. It looks more correct to me to have my tools oriented as they sit in the machine. That may be a moot point in the future, as Machine Simulation should be able to take your code and map it onto the machine you select in machine configuration.

 

Rich,

 

Not sure if you've seen it yet, but we added a Horizontal machine definition to Machine Simulation that will work with Top/Front style programming...

[Richard Thomas - Mastercam UK]

Hi Colin,

 

Yes I've tried using "Horz4Front" (I think that's what it 's called) and it works fine for B0 programming, but as soon as you start trying to machine around the angles in "B" it starts to get itself confused.

 

I think the machine itself was rather grudgingly included at the last minute as a result of a lot of moaning from people like me (and some of the guys above) when Machsim was first integraged in X4. The rest of the horizontal machines don't support Top/Front programming.

[Newbeeee™]

Personally, I do not use the 'Automatic' work offset numbering when I'm programming a job. I set a Work Offset number on each Toolplane I'm using, that way I always know what Work Offset value I'm going to get when Posting. (again, just my personal preference).

 

I don't prog hori's but I really can't see the need for automatic work offset numbering. It seems an accident waiting to happen to me. I think manual is the way to go 100%.

[Bryan Johnson]

using Top/Front for programming a HMC is the display in Backplot and Verify. It looks more correct to me to have my tools oriented as they sit in the machine.

 

In regard to the display, it really only applies in regard to the default gViews, and who uses those for anything?

When i am working in Mastercam, I am most always in a user defined view by way of dynamic rotation. The orientation of the model on my screen has no relation to Top or Front being the B0 view. No one would look over my shoulder and say "Your HMC files look too much like VMC files".

 

My take on this is that the ONLY difference between a typical HMC and VMC, is the axis of rotation. I can not follow the logic in setting up a machine and post definition, and working in an environment where Y axis moves are really Z, and vise versa, and having to switch them back around in the post.

Same thing for Lathe. Instead of working in an environment where X=Z, Y=X, and Y=Z, it would work better if a new GVIEW was made so that you can quickly view the part in the Z/X plane when needed.

 

Helpful tools for rotary programming would be.

1. ability to LOCK the WCS to rotation origin.

2. Have current toolplane clearly represented on screen at its origin.

3. Gviews mapped in respect to current toolplane (quickly look down the spindle / normal to toolplane)

4. A View Manager that does not includes any of the "Default" views, and has quick tool for creating VALID toolplanes for current machine type (rotated about Y or X).

5. Backplot that represent rotary rapid moves.

6. no warning for OFFSET is used in more than one view!!!

 

Most every program I write these days is for a rotary. Most are very simple, but deal with lots of planes and offsets. It seems to me that a few small changes would go a long way in regard to rotary / toolplane stuff.

 

Am I overlooking some simple solutions the these issues?

[Matthew Hajicek - Singularity]

6. no warning for OFFSET is used in more than one view!!!

 

I agree with everything you've said, but this one is particularly annoying. How many extra clicks to clear that, about three or four every time you make a view? There are some places where you can't even clear it, you can only abort!

[Newbeeee™]

In regard to the display, it really only applies in regard to the default gViews, and who uses those for anything?

 

Helpful tools for rotary programming would be.

1. ability to LOCK the WCS to rotation origin.

2. Have current toolplane clearly represented on screen at its origin.

3. Gviews mapped in respect to current toolplane (quickly look down the spindle / normal to toolplane)

4. A View Manager that does not includes any of the "Default" views, and has quick tool for creating VALID toolplanes for current machine type (rotated about Y or X).

5. Backplot that represent rotary rapid moves.

6. no warning for OFFSET is used in more than one view!!!

 

Most every program I write these days is for a rotary. Most are very simple, but deal with lots of planes and offsets. It seems to me that a few small changes would go a long way in regard to rotary / toolplane stuff.

 

Am I overlooking some simple solutions the these issues?

Fully agreed Bryan.

As a noob, I've said it a few times that the whole wcs and view thing takes a bit to get my head around.

As for default views, we use these for straight side 1 / flip side 2 3ax work only. For rotary work, new views every time.

I like your point 4.

I did throw out an idea on the enhancement forum ref views and view manager (but didn't get any comments so here goes).....

 

When we create a new named view in View Manager, would it be possible to have mcam automatically create an icon that displays for that view in a docable toolbar?

When we then want to change view, all we have to do is click the icon?

I realise that this could be ‘a challenge’, especially for the icon so it differentiates itself from one view to the next?

Perhaps user writeable number system (54/55/56 etc) to differentiate G54, G55 etc, or 1/2/3 for OP1, OP2 etc.

Or colour select, so a user can have say green always for OP1, red for OP2 or whatever.

[Tony35]

6. no warning for OFFSET is used in more than one view!!!

 

+1

 

 

How many extra clicks to clear that, about three or four every time you make a view? There are some places where you can't even clear it, you can only abort!

 

+1

 

i know im using the same offset i picked it

 

must be for the 6yr olds

[Mastercam Rookie]

Ok everyone I understand the Top WCS(axis of rotation) Front Tplane(B0), Right Tplane(B90),Back Tplane(B180), Left Tplane(B270), and the program is going off the center of the tombstone, but were would I get the WCS information to enter it in my mastercam, and were would I place that informations. I have notice alot of companies use a G10 X,Y,Z.....which tells the machine where the center of the tombstone is. But again how would I know the center of the tombstone on a horizontal, does that information come with the machine.

 

 

also quick little question, is their any leason out there that walk you thru setting up a toolpath on probing...

 

Thanks!

[crazy^millman]

Ok everyone I understand the Top WCS(axis of rotation) Front Tplane(B0), Right Tplane(B90),Back Tplane(B180), Left Tplane(B270), and the program is going off the center of the tombstone, but were would I get the WCS information to enter it in my mastercam, and were would I place that informations. I have notice alot of companies use a G10 X,Y,Z.....which tells the machine where the center of the tombstone is. But again how would I know the center of the tombstone on a horizontal, does that information come with the machine.

 

 

also quick little question, is their any leason out there that walk you thru setting up a toolpath on probing...

 

Thanks!

 

We normally take a few days on site with a customer to cover something like this.

[jlw™]

That's quite a loaded question.

 

What kind of machine is it? Likely you can get the info from a parameter, if not you'll need an indicator and some one who knows what to do to find it.

 

 

I'm not sure you can make mcam post the G10 line unless you have some custom post work done, any time I define offsets I use sub programs and the machinists probes or indicates to find work offsets.

 

If you don't already have a good foundation of programming 3 axis verticals I recommend as Ron said and have some one come in and set your machine up then go thru the process start to finish in mcam from orienting the part to dnc or how ever you plan to get the code into the control.

 

While there are a lot of sharp guys here on emc the way you asked the questions leads me to think you need more help than you realize.

 

No offense intended but bring some one in to give you a crash course, you'll get much farther much faster.

 

Based on your questions, get the basics then come back and search for probing info. There's a lot here and I have posted a really simple probe program that will demonstrate probing 2 points and a little macro work to set c axis offset.

 

Also, give some specifics about the machine it's likely there is some one here who knows exactly what parameter to get the center of rotation from.

 

Good luck!

[Mastercam Rookie]

That's quite a loaded question.

 

What kind of machine is it? Likely you can get the info from a parameter, if not you'll need an indicator and some one who knows what to do to find it.

 

 

I'm not sure you can make mcam post the G10 line unless you have some custom post work done, any time I define offsets I use sub programs and the machinists probes or indicates to find work offsets.

 

If you don't already have a good foundation of programming 3 axis verticals I recommend as Ron said and have some one come in and set your machine up then go thru the process start to finish in mcam from orienting the part to dnc or how ever you plan to get the code into the control.

 

While there are a lot of sharp guys here on emc the way you asked the questions leads me to think you need more help than you realize.

 

No offense intended but bring some one in to give you a crash course, you'll get much farther much faster.

 

Based on your questions, get the basics then come back and search for probing info. There's a lot here and I have posted a really simple probe program that will demonstrate probing 2 points and a little macro work to set c axis offset.

 

Also, give some specifics about the machine it's likely there is some one here who knows exactly what parameter to get the center of rotation from.

 

Good luck!

 

 

Thanks for the reply JLW,

 

 Just to let you know what I was thinking of doing is touching off the table to find the center of it, before I add the Tombstone on...but could you awnser this question maybe, let say I got the WCS information I would Like to enter, were would I add it to?

[jlw™]

To the offsets page in the control unless you want to program in machine coords.

 

What kind of machine/control is it?

 

Your reseller will have plenty of tutorials for free simply by asking.

[RaiderX]

one method that I have seen is g10 line is hard coded in the post as machine to cl rotation and all programming was done relative to cl. just one approach of many options.

[Mastercam Rookie]

To the offsets page in the control unless you want to program in machine coords.

 

What kind of machine/control is it?

 

Your reseller will have plenty of tutorials for free simply by asking.

mazak/mazatrol...just to let you know im a student at a college, for some reason the dont have it...and not to be rude but teacher is full of it...

[Mastercam Rookie]

To the offsets page in the control unless you want to program in machine coords.

 

What kind of machine/control is it?

 

Your reseller will have plenty of tutorials for free simply by asking.

JLW,

 

 You know how sometime you might over think yourself to figure out a problem I think this was one of those times, I figured out what my problem was and corrected it... thanks everyone for your help

[jlw™]

When you get ready for probing let me know, I can help you with that Mazak.

[BenK]

mazak/mazatrol...just to let you know im a student at a college, for some reason the dont have it...and not to be rude but teacher is full of it...

With all due respect if your a student how would you know if your teacher is full of it?

 

Many of the things people have been pointing you to are beyond what you should be worrying about as a student and if you told us that up front we could have answered your questions better. Let's start at the beginning. Do you know how to set an offset on the machine? The offset register is based off machine coordinates and you don't put that information into your CAM file. Next do you know how to find center of rotation?

 

You're asking about step ten when you should be asking about step one. Without the basics everything else is going to be pointless.

[Rocketmachinist]

mazak/mazatrol...just to let you know im a student at a college, for some reason the dont have it...and not to be rude but teacher is full of it...

What school are you going to?

[Müřlıń®]

I set up my machine as you are looking at it from the ceiling down. WCS top/front

 

then the front view is looking through the spindle.

 

B0 can be anything.....it depends on machine and where they want to set it..

[Rocketmachinist]

One question that I have been wondering, we just got our ec-400 and looking into the different techniques to program it.

 

I undertsand one way to program it is to use the g54 g55 g56 etc and just re touch off each part depending on the angle.

 

So g54 of the part will be a (just for example) in the offset table x0. y0. z0. B0. for part 1. But if I want to do the right side of the part it will be something more like g55 x-6. y0. z-6. and B90. This works if my parts are square and I am doing one part at a time and only working on 90 degree faces (its also time consuming).

 

The other way to to use g54 as my center of tombstone rotation and then probe all my parts and shift them in mastercam to where they are relative to the center of rotation.

 

It seems to me like there would another way where the controller takes over and will keep track of the part rotation g10 I hear. But the books have no depictions on how to use it.

 

Am I missing anything. I have read many forums talking about top/front which makes sence to me. But, what are you using for your wcs? The edge of the part? Center of Rotation?

[Müřlıń®]

WCS is Top.....

 

one G54 where center of b axis on top of the rotary table....

 

Everything else comes out in the wash...

[jlw™]

One question that I have been wondering, we just got our ec-400 and looking into the different techniques to program it.

 

I undertsand one way to program it is to use the g54 g55 g56 etc and just re touch off each part depending on the angle.

 

So g54 of the part will be a (just for example) in the offset table x0. y0. z0. B0. for part 1. But if I want to do the right side of the part it will be something more like g55 x-6. y0. z-6. and B90. This works if my parts are square and I am doing one part at a time and only working on 90 degree faces (its also time consuming).

 

The other way to to use g54 as my center of tombstone rotation and then probe all my parts and shift them in mastercam to where they are relative to the center of rotation.

 

It seems to me like there would another way where the controller takes over and will keep track of the part rotation g10 I hear. But the books have no depictions on how to use it.

 

Am I missing anything. I have read many forums talking about top/front which makes sence to me. But, what are you using for your wcs? The edge of the part? Center of Rotation?

Is this a mazak? I would use g68.2 to shift. When you rotate as you say, the shift will account for the devation in rotation and the center of rotation. If you only have one part I'd use g54.4.

[Rocketmachinist]

Not Mazak, Haas

[mkd]

only the new 750 has DFO.

 

ec will need to go off centerline just like the verticals.

or get fancy with some macros to calc and use g10 to set offsets.

[Rocketmachinist]

^^ Thanks so much. I have been trying to nail this down in my brain for months.