What's new
What's new

Programming multiple parts per fixture

Cole2534

Diamond
Joined
Sep 10, 2010
Location
Oklahoma City, OK
Hello,
I suspect this comes down to a mixture of personal preference and resource limitations but I wanted to ask anyway.

If you're milling multiple identical pieces per fixture, do you program each piece as a new fixture offset or set the fixture as one offset and have multiple entities in the model? It seems like the biggest decision is whether you want to make individual tweaks in the control or in the model, but maybe I'm missing something.

Are there distinct advantages to either method and which do you prefer?
 
Hello,
I suspect this comes down to a mixture of personal preference and resource limitations but I wanted to ask anyway.

If you're milling multiple identical pieces per fixture, do you program each piece as a new fixture offset or set the fixture as one offset and have multiple entities in the model? It seems like the biggest decision is whether you want to make individual tweaks in the control or in the model, but maybe I'm missing something.

Are there distinct advantages to either method and which do you prefer?

I use a combination of both. For example, might lay out multiple pieces for a sanity check, then program one face pass (for example) setting stock up for G54 only. Then I might transform the spot/hole drilling ops. Depends entirely on part and features IMO.
 
Reason for my Q was that I need to drill/tap Al bars in the vise, no critical features or dims. In the manual mill I'd line them up, locate one hole, and then offset by the spacing. In the CNC, the vise is already a fixture so just model up however many pieces fit in the vise, or do them individually.

I think it depends on how picky the parts are, I'd rather make individual tweaks for location in the control rather than the model.
 
advantage with a different work offset for each part is when each part is probed and different work offset used for each part. the probing can get exact location on specific features like a bore or specific surfaces
....often parts spaced the spacing is not exact and can vary .001 to .010" if edge locators are not exact in position or torque used not exactly the same or even uneven temperature control, probing will give a more exact current position of specific features
 
It depends really.
Are these 1st op parts where you're qualifying the outside to make sure the holes will be in location?
Or are they 2nd op parts where a finished edge is up against a stop?
If you're locating a finished edge up against a stop I would go with separate work offsets.
If it's raw stock, just 1 offset will suffice.

I do both, sometimes in the situation above, or how I'm feeling that day.
 
As long as the quantities support it I always program 1 or 4 parts then shift the coordinate system to make more, usually with fixture offsets. Of course, the best answer to your question is "it depends". For lower quantites I just make one part at a time since I make them on a fast drill/tap mill, another important detail to how to program is what are you programming for.
 
Personally I like to use a separate work offset for each part. Just because I like to have the most control over my parts. But as stated above if it's the first op it's usually not an issue to just pattern out the toolpaths on the CAM side.
 
If I am cutting fixtures (or soft jaws) and putting the parts in them, then I'll use pattern outputs from CAM and a single WCS zero since the machine will repeat. If it is something like vise work I use multiple WCS. If I have probing this also changes things since I will generally probe certain types of features on a machine that won't be slowed down much by it (Speedio, Robodrill, etc.) for vise work.
 
As long as the quantities support it I always program 1 or 4 parts then shift the coordinate system to make more, usually with fixture offsets. Of course, the best answer to your question is "it depends". For lower quantites I just make one part at a time since I make them on a fast drill/tap mill, another important detail to how to program is what are you programming for.

I usually do that, but I'm trying to train myself to step back from the machine so I can multitask.
 
You also could try G52 local coordinate system with each shift calling a subprogram for each machining operation. Only have to set one work offset that way, and spacing can be easily altered by the value on the G52 line.
 
Generally speaking, I use a different coordinate system for each loose piece of material. If I am making 2pcs. from one block then they will be modeled and programmed together in one system.

Sent from my SM-J737V using Tapatalk
 
When I program multiple parts I like to use a MCS for each part unless multiples are being milled from one block, as cmainman mentioned. It is desirable to use multiple MCS if you are nesting parts with multiple orientations and non-nominal spacing. In those cases it's nice to have your cam system use one program and apply to to all MCS's regardless of how and where the part are situated and still be able to do full tool path checking and simulation. The icing on the cake is the ability to deviate from instanced tool paths and tweak individual parts if needed but still have full associativity and be able to revert back to the instanced paths if needed. I love that feature of NX. On a tangent, another cool feature which comes in handy is the ability to use an IPW (stock model for the MC guys) on various parts with MCS's all over the place. Again with full associativity, gouge checking and simulation.
 
I vote for compact code, one program called multiple times with datum shifts or offsets or whatever. It ensures that the same code is run on each part.

I concur. Also safer. One local drawing. One local program. Once proofed you can dance it around the stock and/or machine any way you want using on the fly G10 offset changes or simple work coordinate changes or both. I'll create programs that have all the additional part program calls block skipped out. Button in... one part. Button out... many parts.

Dave
 
If I am cutting fixtures (or soft jaws) and putting the parts in them, then I'll use pattern outputs from CAM and a single WCS zero since the machine will repeat. If it is something like vise work I use multiple WCS. If I have probing this also changes things since I will generally probe certain types of features on a machine that won't be slowed down much by it (Speedio, Robodrill, etc.) for vise work.

I do the same. Both ways depending on the setup or qty. Multiple or perhaps different vises I program one part and the post spits out sub calls and separate WCS for each.

Dedicated fixture? Array or pattern in CAM and make it one big program. One offset per group of parts.

Keep in mind the amount of tool changes with some of these suggestions.

Either way you can still minimize toolchanges. In both methods each tool is run through the whole lot, before changing to next tool.
 
Keep in mind the amount of tool changes with some of these suggestions.

The program style I speak of has the exact same amount of tool changes regardless of how many parts. The block skipped blocks that call for additional offsets or parts to be made are included in each tools' programming.

Dave
 
Keep in mind the amount of tool changes with some of these suggestions.

absolutely

It does depend on machine tool change time, but most of my programs consist of a series of subprograms then datums shifts and label calls[heidenhain speak]

I tend to write them as a single position then label them after so the program rarely begins at block 1, just a note at the beginning saying 'starts ad block 456'

keeps it so I can run one part if need be.
 
Pros:
- Fewer tool changes
- Potentially less air cutting from fewer lead-ins/outs
- Easier to re-run finishing ops for high accuracy features
- Higher density fixtures are possible

Cons:
- Tweaking programs in CAM may require reselecting a lot of geometry
- Programs can be much longer, a problem if your machines are memory-limited
- Proving out programs can be tiresome (babysitting a much longer cycle)

So we split the difference.

On a 4-sided tombstone in an HMC, running identical parts on all faces and multiple parts per face, we machine all identical parts on one face simultaneously. Then index 90, run again, rinse and repeat.
 
It is too bad autodesk is ruining FeatureCAM. It has the best multiple fixture function I have seen in any CAM system.
I have not seen everything. But, I use the hell out of FeatureCAM's "multiple fixture document".
 








 
Back
Top