What's new
What's new

Deckel fp4a diagonal machining

Harri89

Cast Iron
Joined
Nov 21, 2016
I need To drill and tap holes to 18 pieces of aluminium angle bar which is longer (711mm) than my Deckel FP4A x axis travel but it can be done diagonally with x and y axis.

How should i approach this and program the machine? Can i locate edges/corners with edge finder and get the points for the control so it can determine the angle it is clamped to?

Or do i need to do it manually and calculate the angle and use coordinate rotation g code?

The machine is with Grundig contour 3 control which is similar to Dialog 4.

Thanks! :)
 
program your holes in the control, mount a sacrificial "pallet" on the table where the work piece will be located, offset X by x amount, drill starting and end holes in the sacrificial pallet, use those holes for reference to fix your work piece to the table (or that sacrificial pallet), undo the X offset, make your parts
 
Not sure you have the travels to run this diagonally...Looks close to me.
Seems as you will need a minimum of 440mm of cross travel to fit your length if your "X" has 550mm travels. (not sure about the FP4A)

To me the operative word here is "drill" seems that high accuracy here is not required.
Personally i would run this job doing each angle 1/2 at a time....setup two qualified vises on your machine and use them to hold the angle.
Drill and tap one half of each angle, move in the vises , use the last hole drilled and tapped as the datum for the next set of holes.
Use a threaded plug with a good center hole to run into the threaded hole to spot the spindle in order to drill the next half.....

If you don't have dual vises, then a piece of plywood down on the table and locating posts to butt the angle to for repeat positioning.
Hold down clamps to hold the angle against the plywood....

Cheers Ross
 
X travel is 560mm and y 500mm, these are for accuride heavy duty drawer slides. For each angle bar 4 x m6 thread, they will be fixed togheter with countersunk bolts. There are countersinks in the drawer slides, so There isnt much room for error to Keep the angle bars straight.

I can use spot drill and carbide drill for the holes or drill straight with carbide...
I dont have two matching vises.
 
. For each angle bar 4 x m6 thread, they will be fixed togheter with countersunk bolts. There are countersinks in the drawer slides, so There isnt much room for error to Keep the angle bars straight.

All the more reason to run them straight...easier to gauge if the parts are sitting straight with the machine....could even indicate them if needed.
Simpler, less chance of any error, and easier to see if something does not look right.

However if you wish to use the control to run the parts at an angle , think you can use G56. (absolute rotary offset of the coordinate system)
You can use an angle of rotation ,or a displacement of two points to define the coordinate shift.....
Once the shift is defined, you can drill the holes by simply programming the distance between the holes as though the part was sitting straight. ( straight X move)

You will still need some setup to locate your parts and you will need to accurately calculate the angle the part is sitting at or the position of the first hole referenced to a start (pole) point....
Additionally, think you will need to be careful of any locating errors (start point). If i understand the job there are right and left rails, so any error in initial position will be double ,(right /left)
So you may need to run the parts starting at opposite ends (right and left) so that any error in the overall length of the rail will be cancelled.

Also, you will need to position the part with its center of length pretty close to the middle of both axis travels (X,Y).
Don't forget to cancel the shift (G53) before doing any additional positioning moves.

Cheers Ross
 
You don't need two matching vises. You can use any two vises that have the same height which you can do with custom parallels if necessary. You could also do it on the table with a sacrificial piece underneath as Ross suggested.

I've done linear bolt patterns on rails 5ft long with my FP1.

1. Drill hole and retract to remove chips.
2. Drop drill into hole with quill.
3. Loosen vises.
4. Move X to locate new position, moving part in vises.(table moves, part remains stationary)
5. Tighten vises
6. Retract drill
7. Seat part
8. Move to next hole location
GOTO step 1

If you are going to tap the hole, suggest to do it after step 7.

No fancy CNC or rotated coordinate space but it will get the job done quickly with a minimum of fuss.

Teryk

Sent from my XT1710-02 using Tapatalk
 
How do you get done some irregular parts that need machining afterwards, what are your methods to know its position?

I assume that if you want the part shape to machine you need a probe and machine with specific software?
 
How do you get done some irregular parts that need machining afterwards, what are your methods to know its position?

I assume that if you want the part shape to machine you need a probe and machine with specific software?

I'm not sure if your question is directed at me or not. Either way, I think you may need to try again at asking the question, perhaps with an example. It is hard to determine exactly what your question is.

If you are asking how to locate features on irregular parts, the general process (in very simplified form)is to:

1. measure the part in question and perhaps draw it up in CAD
2. Establish datum features which can be located on the physical part and add them to the model. You need enough datum features to eliminate all 12 degrees of freedom.
3. Create measurements from those datums to the features you are going to machine in your CAD model.
4. Place the part in the machine and use physical stops, dial test indicator, edge finder or probe to locate your datum features and establish your part zero
5. Machine your new features.

If you really wanted to machine your rails at an angle, I think your best bet would be to draw it up in CAD at an angle so that you can determine your hole locations as well as the locations of three pins that you will use to locate the rails in X and Y as well as establish the rotation in the XY plane. You could also do this by hand with a bit of trig if you like that kind of thing.

Make a fixture plate using those pin locations and an easily located part zero such as a corner feature, boss or bore. Clamp your part onto your fixture plate, using the locating pins and machine your features using the dimensions from the CAD model.

Sent from my XT1710-02 using Tapatalk
 
There are tons of methods that one can use to re-locate a part that must be moved to complete its finished machining.
Generally you need two reference points (position and orientation).
These can be reamed holes, center drilling, edge features or part features (pockets etc), tool makers buttons....
If not two reference points, then a single reference, and some fixturing method of aligning one side of the part....
Soft vise jaws machined to accept different features of the part also can work.

The thing in all this that saves immense time and work is a drawing program.
If you have two reference points that you can indicate , and you know where they lie (accurately drawn) within your part profile, then you do not need to really orient the part.
Simply find the points , enter their location on your drawing, then move the drawing till the original drawn points agree with the current measured points, the result will be a part profile
that is now aligned, and can be cut without worrying about how exactly it is pointing....
Much easier to move a drawing on the computer than mess about indicating edges and the like.

Don't need a high powered CAD system to do this...For years i programmed my machines using a "demo" version of "SurfCam". Could draw and manipulate geometry. Did everything to size and all, but
was restricted to not being able to post process the tool path, so the program would not write code directly.
Not a problem, The program could solve for circle and arc start and end points, line start and end points, which allowed me to solve all geometry problems and enter the information into my MDI programs....
Worked a treat, with zero expense.
When i got better established i bought the full feature 2 1/2-D program, which i was by then pretty experienced at using.....Some time later i upgraded to a full 3-D version, which i still use today.
My point is that there are solutions out there that can be found that don't require cubic cash to enhance your work.

Cheers Ross
 
That Haas probe flick is pretty usual stuff....
Really not applicable to your Dialog control....
You need a real probing cycle to do what they are showing....
The accuracy and repeatability of a probe is dependent on approach and touch off at a constant speed (power). Then the probe trigger is fedback to the control, where values are set using macros.
More or less beyond the Dialof4 capability....

If i was making that part i would do the holes first in my part blank, then use the holes to align the part via fixture, no prob needed....
He has everything he needs there, just a better holding setup....Single point clamp is asking for the part to twist under machining....
Cheers Ross
 
If the part fits diagonally, then I would use Ross' suggestion in post 5. Don't forget that you have three planes to work in, so even if it does not fit in XY plane it might fit in XZ. Since Dialog supports polar coordinates, the change of axis command is extremely useful. Let the control do all the calculating work, since after the change of axis, all your moves will be relative to the new axis. It is one of my favorite ways to use Dialog. I don't have a toolmakers table on my FP2NC, so my Deckel rotary table stays installed most of the time, making it easy to dial in alignment with the axis.

Dialog 2 only supports a single change of axis command at a time. i.e. you cannot rotate XY plane 10 degrees and then rotate XZ plane, you will get an obscure error on the control panel. I don't know if that limitation applies to Dialog 3 or 4, but it would be useful to know.
 
That Haas probe flick is pretty usual stuff....
Really not applicable to your Dialog control....
You need a real probing cycle to do what they are showing....
The accuracy and repeatability of a probe is dependent on approach and touch off at a constant speed (power). Then the probe trigger is fedback to the control, where values are set using macros.
More or less beyond the Dialof4 capability....

If i was making that part i would do the holes first in my part blank, then use the holes to align the part via fixture, no prob needed....
He has everything he needs there, just a better holding setup....Single point clamp is asking for the part to twist under machining....
Cheers Ross

I assume this kind of stuff is impossible in dialog manually with 3d haimer example?
 
Using a "Haimer" style Tastar can give good position data...but its all dependent on how its used...The gauge needs to be fitted to a dedicated tool holder and zeroed to that holder(calibrated) .The Haimer style indicator (which i like) is also dependent on movement.
To get repeatable results that are accurate you need to approach the zero point at a constant feed rate and stop when the dial exactly hits zero....
Herkey,jerky moves, start ,stop or a change in rate will all affect the indicated zero position.

The human element here can create some errors unlike a true probe running under automatic probing cycles (CNC) where everything become very consistent.
A Tastar will give position data of any singular point on a part profile. For this to be usable you need to have a datum on both the part and drawing from which you can solve for the location of any testing point.

Cheers Ross
 








 
Back
Top