could some one explain this

[jlw™]

Well, I've been using mcam for just under a year now.  Never once used this, could some one give me a run down on it:

 

[The Cathedral]

The reference points are points you use to start and end your toolpath. For example, if you have a really long tool that you need to move away from a fixture before you toolchange, you would put that point in the "retract" dialog box.

 

The home position, I have never used. I suppose how your machine and post operates would dictate how you would use it, but on our Doosans and Okumas we never use it.

[Colin Gilchrist]

As Cathedral mentioned, the "Reference Points" let you add an "initial start point" and a "final retract point" to any toolpath. This allows you some flexibility in getting the tool into and out of the cut. The "Reference Points" are a must for Lathe ID work, as it ensures that your tool clears the bore, before it tries to go to the tool change position.

 

The "Home" coordinates allow you to enter a distance from your Work Offset location, back to the home position of the Machine. This feature can be used for several different things, however, here is the "default behavior":

 

With Mastercam, there are basically two different ways to set your Program Origin. One way (and by far the most common and modern), is to use a "Work Offset". To use Work Offsets, you must set 'misc integer #1 to a value of '2'. Then you should set your Work Offset value in the Planes Manager.

 

If you set "Misc. Integer #2" to a value of '0' or '1', then you get a "G92" at the start of the tool, which is used "in place of" a Work Offset.

 

For G92 "Home Position" values, you are relying on the Operator of the machine to position each tool in MDI to the correct Machine Position, before they hit Cycle Start.

 

When I worked at Boeing, we had a bunch of ancient Gantry style 3X Routers. Each machine had a set of Tooling Holes, with steel bushings, on a 10" grid across and along the machine table. This would allow an operator to load many different fixtures on the machine, and simply jog the machine to a "known start location". We used a "Pin Check" to ensure that the machine is starting in the right location. In our case, our "Home Position" was always -30., 0, 3.0. So that means the operator would jog the machine to the pin hole that is "negative 30 inches" from where the fixture is pinned (located). The operator would jog the machine to the pin hole that is 30 inches away from the part pin location, and load a tool holder with a gauge pin. Since the machine should now have a pin in the spindle, the operator would also put a pin in the table at that hole location. A bushing is slipped onto the "Home pin" prior to starting the process. So when the "Pin check" comes up, the operator then slides the bushing up from the Home Pin, onto the Tool Pin. That gives them a quick check to be sure the machine is in the correct position before hitting cycle start.

 

The point is that our Program Headers always used "G92" for setting the Home Position, and the output from the post is a G92 line, with XYZ values that are entered on the Home Position page. One thing to note is that the Home Position, is by default, also the "Tool Change Position" used in Backplot/Verify. So if you put values in there (relative to your Work Offset), you will see the tool move to that position when changing tools...

[crazy^millman]

In Multi-Axis Toolpaths these are very useful. Like Colin Said a must for Lathe ID work.

[jlw™]

When will it go to these points? In rapid? I use clearance all the time, will it rapid to this point then to the clearance point, run the path, then to retract point?

[crazy^millman]

Sometimes I will use them and no Rapid or where I want Rapid at a certain distance while doing work on a face of a tombstone, but the go to a different distance for the start and end of a group of operations. Let say you have 20 operations for a face of a Tomb stone. The 1st one can have the Approach and the last one will have retract. Now you get a Certain distance for the approach and a certain distance for the retract, but then get the small rapid you want for all the other operations without having to have all the rapids out to that extra distance you want to be for indexes.

[jlw™]

Ah, now I see. How freakin useful this will be!

[Fred @ Slate Industries]

Onezies and twozies I make Dummy moves.

I just make a "Fake " drill point etc.

operation to get the tool up and around and back from the

Bogey man. Conversational Lathe action, I key in the home ref #'s so the tool just makes it

Between the stock and the Center/Tailstock .

 

HTH

[The Cathedral]

We run parts on a horizontal where we have to insert bronze bushing. I have the toolpath programmed using point toolpaths, but I set the approach and retract points at a position near the door, so the operator can open it up, slip on a bushing, and then the machine inserts it.

[jlw™]

Nice! I've wondered how to do stuff like that in mcam! Can you make it rotate BC in this move? Say, I want to position it at the door and the roll B90 so they can flip inserts?

[Colin Gilchrist]

Nice! I've wondered how to do stuff like that in mcam! Can you make it rotate BC in this move? Say, I want to position it at the door and the roll B90 so they can flip inserts?

 

 

No, you cannot change Planes with a Reference Point, and Changing your Plane is what causes Mastercam to calculate a Rotary move.

 

To do what you are asking for, you are best served by using Manual Entry to input the G-Codes and M-Codes in the exact sequence you want, or to use the "Point" operation. The "Point" toolpath does let you select a Tool Plane, so potentially this would work for allowing a position and rotation to occur. In the Point Operation, you can use "Canned Text" to output pretty much any NC code you desire. M00/M01 are setup to be output through Canned Text by default, so you don't have to do any post mods to get a Machine Stop. For other options, you'll need to edit the Canned Text output. (That may be possible in your Postability post, without having to get Dave to make the edits for you...

[jlw™]

I have been using manual input.  Esprit has a "tool change" path that runs it to any position you want in g53 or an offset.  I figured mcam had the same some where and i just haven't ran up on it yet.  The point path would probably get what i want.

 

Mazak has the lovely TPS so that's how we do it now.  I usually use a manual entry and mo with a message to check the tool.

[jlw™]

Bump, got another question about this and I'm at home now so I can't post and check.

 

But I'm curious, are these ref points relative to WCS or T/CPlane?

[Newbeeee™]

Bump, got another question about this and I'm at home now so I can't post and check.

 

But I'm curious, are these ref points relative to WCS or T/CPlane?

Never thought of this but it must be from T/C Planes.

We use them for 4th Rotary work (talking vmc), so we can retract high enough for an index (just a Z retract) or for a toolchange (Z up and X move).

I'm thinking we did a post mod (can't remember though) so Z always moves first and next line is the X move so we don't get a diagonal move.

It works real well.

[Colin Gilchrist]

I believe the Reference Points are Tool Plane based, but the Home Position might be relative to the WCS.

 

One thing you'll notice (if you turn it on) is that Home Position should be where the Tool starts from and goes back to for Backplot. (there is a switch in Backplot to enable this.) It is really handy when you need to see the tool move back to the Tool Change position, and start from that point again for the next tool.

[Jayson Kramer]

I use the Retract one for example with one of my customers as they have a small trunion on the table to the right. with a part loaded this can be tall.

So i but on the last of just before a tool change a retract of X-10.00 this moves the table over so it can do a tool change safely. between ops.