Harmonic analysis

[krishi1978]

Hello all,

as a part of my work i need to work with milling simulation. And the analysis type is "Harmonic analysis". Can anybody suggest how can i proceed for this and which software would be ideal.

thanks,

krishi.

 

[gurmeet2003]

Krishi,

Harmonic analysis generates the response transfer funciton. For a specified load amplitude and location, you can find out the response at another location over a spcified frequncy range. The input is the force amplitude and the output is a plot of response as a function of frequency. You also need to specify the damping.

Both ANSYS and ABAQUS can do this analysis. I prefer ABAQUS.

Thanks,

Gurmeet

 

[krishi1978]

gurmeet,

thanks for ur reply. Here i would like to use ANSYS..coz in our company we have license for ANSYS only. with abaqus i worked on the vibration analysis when i was in university..anyhow...the model for the milling simulation...which would be better...2D model...or the other ideal model....any suggestions....

thanks,
krishi

 

[rob768]

3D beam elements and distributed masses.....Very efficient and accurate

 

[krishi1978]

hello rob768,
thanx for ur hint. I am working on it. Could you plz tell me elements would play any imp. role in this analysis...

thanks.
krishi

 

[rob768]

Model the steel structure with appropriate beam elements. Model masses of motors, rollers and other components as mass elements, and connect those parts through rigid elements to the steel structure. Use enough elements to realistically represent possible mode shapes (modifiy when an unexpected mode shape appears, or if in doubt). Be careful on modelling connections (bolted, welded, plates)
The basis idea is the represents stiffness, mass distribution and possible deformations as accurate as possible, without concerning on how it looks, or things such as stress concentrations.

Note: a modelled construction is usually considerably stiffer than the real thing, especially due to the representation of connection poinst suc as welds or bolts. Actual frequencies will usually be somewhat lower than those calculated.

 

[krishi1978]

hi rob768,

thanks a lot for ur suggestions. I understood what u suggested. But for me the problem is, i am unable to model the task. i.e , As i explained earlier, i need to simulate(harmonically) a milling cutter with 4 inserts. I am not getting the idea how do i model it in ANSYS. If you have any idea, could u please suggest something regarding this.

thanks,
Krishi.

 

[cbrn]

Hi,
from my point of view, the load on your milling structure should be divided into two parts:
- constant load: it is the force, normal to the mill's axis, generated by the advancement of the mill into the machined piece. This force could have any direction if your milling machine is multi-axis, so you should first think about which is the direction where the forces are expected to be higher, or where the structure is expected to be less stiff. With this force(s), run a static analysis with "prestress effects -> ON" so that you generate a load vector for the subsequent harmonic response analysis.
- pulsating load: it is the quota of the constant load which varies because of the "teeth-passing". There are several theories of milling which can predict (but with a considerable uncertainty) the milling force as a function of time (periodic), known the feedrate, the pass depth, the spindle speed, the number of teeth, and of course the combination of mill material / machined material.
In your case, the pulsating load will have a frequency of 4*n, where "n" is the spindle speed and 4 is the number of your tool teeth. You can also input a range of frequencies if you want to explore the behaviour at different spindle speeds, but be careful because you should vary also the magnitude of both the constant and pulsating part of the milling force (you can do this with tabular loads, but I think it wouldn't be so simple...).
- run the harmonic response analysis with the "prestress effects -> ON" and by loading the load-vector previously calculated.

From a modeling point of view, the mill will be a beam or a shaft element, at the end of which you will apply the force.
Of course, if you know for sure other sources of harmonic excitation (motor harmonics, etc...) you'd better include them as well. But in an harmonic analysis in Ansys, every point of excitation receives the same periodic force, so you will have to run several loadcases and then combine them together in some way.

Regards

 

[rob768]

I have no idea how to define the loads in ansys, but i think the post above tells it all.

 

[krishi1978]

Hi cbrn,
Thanx a lot for ur detailed reply. You explanation is really helpful. But coming to me, the problem is not to define the loads and forces. I already finished everything on the paper. With the help of stability lobes i can finish my work. The exact problem for me is, how to model the milling cuttter and work piece when are in action(to mesh the models). As everybody knows, Milling cutter is round, and on the circumference inserts will be placed. And it moves on the cutter, either axially or radially. It is possible to move either the milling cutter or the work piece. In my case i can take any of these . But the modelling idea, my small brain is not getting. Do i need to take complete model, like a 3D CAD model of the cutter with insert on it or is there any trick in Harmonic analysis. If you have any idea please suggest to me.

thanks,
krishi

 

[cbrn]

Hi,

I think you could super-simplify your work if you model the entire milling cutter + inserts as a "cylinder" (i.e. a succession of beam/shaft elements.
In fact, I don't think your concern is about harmonic response inside the milling cutter, but how cutting forces can ingenerate vibrations in the milling machine.
To over-simplify, you could also take the milling cutter completely out from your problem and apply the loads it generates directly at the extremity of the spindle (in its turn, modeled as a beam, a pipe, or a combination of these, or even modeled with 3D elements if you want to be super-accurate).
I wouldn't go and analyze the whole milling machine in 3D if I could build up a simplified model.
Now I realize that your problem is perhaps different again: if you want the cutter to INTERACT with your workpiece, then it becomes VERY difficult and you will be forced to go into:
- non-linear transient analysis
- death-and-birth of elements (as during cutting, material is removed from the workpiece)
Never done that before, so I couldn't suggest you any more.

Regards

 

[krishi1978]

Hi cbrn,
as u guessed my analysis is linear forced vibration analysis. Actually if i know correctly, harmonic analysis means linear transient with either free or forced vibrations. Anyway, i know about my task perfectly, i.e its linear forced vibrations. No doubt in that. So u suggested that, there is no need to go for a 100% actual 3D milling cutter model, rather i can use or assume, milling cutter as a cylinder(beam or shaft) elements and work piece as normal steel material(plane stress(axissymmetry elements) elements, is this ok in my case?). The very important is i need to specify the direction of Fn,Ft and sinusoidal load. With your suggestion i understood this. If this is correct, its nice. If not, you can give me ur ideas.

thanks,
krishi.

 

[cbrn]

Hi,
there is still one point in your problem that I can't capture: it seems, but I'm not sure, that you need to investigate not only the response of the milling machine but also the one of the milled piece; moreover, do you need the milled piece in order to investigate an "overall" vibrational problem, or do you specifically need to investigate how the mill is cutting into the piece? Let's call these two cases "case a" and "case b":
- case "a": that's as you say. The milled piece will serve you to apply the correct distributed mass over the system, the milling cutter as the correct application point of the force(s). Remember that HARMIC is only in linear field: if you have non-linearities such as contacts, unidirectional restraints or so, you will have to shift to TRANS. Moreover, HARMIC is assuming a single force module with sweeping frequency, applied to as many application points as you want, but it's always a single force module. If you have constant + harmonic forces, you'll have to do 2 loadcases and then combine them by post-pro.
- case "b": wouldn't know exactly how to do this, although I know that "somebody" has already performed analyses like that. Probably contacting Ansys support directly could help, at least for receiving some references or case-studies.

Regards

 

[krishi1978]

hi cbrn,
my task is to investigate regenerative chatter in the milling cutter. Regarding this i am reading lot of journals and what i understood is, at certain spindle speed and cutter speed(as we all know, in milling either of one is rotational or both r rotational), the vibrations will be developed, because of which, the surface finish of the work piece is not good and it also leads to the tool insert breakage. First i need to investigate this vibrational occurance by simulating both evenly pitched and differential pitched milling cutters separately. Depend on the results, i need to minimize the geometry of the cutter(which produces the min chatter, that i need to use to modify the geometry) so that regenarative chatter will b less. I hope u understood what exactly i want to do. However ur suggestions are really helpful for me and always welcome. Thanks for that.

regards,
krishi.

 

[cbrn]

Hi krishi,

well, it's a bit difficult... ;-) First of all, I would not depart from your original idea and, since you know what it takes as regards forces etc, I'd try and see if the machine + workpiece system has one or several peak response(s) at some frequency(ies) in its target working field. For this, no exam of the "in-deep" cutting process is needed. This should help finding out combinations of regime / feedrate which are to be avoided (because otherwise the machine would encounter a "resonance").
I forgot to ask you if you work "on the machine side" or "on the tool side"... Anyway, the second step would be to simulate the cutting process: in this case, only a very small model would be necessary, but in full-3D: the mill-tool and a part of the workpiece. As boundary conditions, you would have equivalent stiffnesses calculated with what we could call "the complete, simplified model". There must be a way to simulate high-speed fracture ( = milling process, as well as lathe-turning etc...) with Ansys, but it's a completely different field from mine and I wouldn't know how to do it (should have something to do with "death-and-birth" of elements, I suppose, as well as with remeshing and so on...).
I hope these few considerations can give you some ideas anyway...
If you are successful with the full cutting simulation, do tell Ansys and you will most probably be registered among the "success stories" of the product, which is a good advertisment both for you and for Ansys: that's why I'm convinced that Ansys' technical staff will be ready to support you with this particular, very interesting task.

Regards

 

[krishi1978]

hi cbrn,
Thanx for ur reply. And coming to our topic discussion, as i explained in my previous post, it belongs to "tool side" only. There is nothing to do with machine. However, i hope that i will finish this task sucessfully with in 3 months. And as u suggested, i will try to contact ANSYS support people once i will get the new license.
Thanx once again for ur replies and always welcome for ur valuable suggestions.

regards,
Krishi

 

[krishi1978]

Helo cbrn,and to all other co-enginners

in your reply you mentioned that, one case is with vibrations in the milling machine. And you explained that, i need to model just the spindle and at the end of that, i can apply the force which is equal to the force generated by the cutter(this is case where i will exclude the milling cutter, to super simplify my model). I would like to know some more detail explaination for this case. Please can you provide me with some more info regarding, modelling, forces and the other important things.

My self and my team mates discussed about both analysis(machine vibration analysis, tool-work piece interaction) and decided to work with this first. So please let me know about all your suggestions.

thanks in advance,
Krishna.

 

[cbrn]

Hi krishi,

it's difficult to figure out exactly how your dynamic system is made, without seeing it, but let's try to build up something:
- machine+tool+workpiece close a kineto-dynamic "chain", i.e. a forces' loop. Somewhere in this loop you have to put your excitation frequancy(ies).
- you told that you know from calculation the forces which are ingenerated between the workpiece and the cutter during milling: so, the node-point for applying these forces will be the end of the tool where it comes into the workpiece.
- the tool can be simulated by a beam with circular section
- the spindle can be simulated by a succession of circular beams or pipes
- you can go on discretizing the machine with beams / trusses as finely as you want. Note that if in some regions you feel more comfortable with 3D elements, you can incorporate them with no problem, but be careful with what follows...
- at a certain point, you will come to the machine's basement: there, an element able to correctly capture a uniformly distributed mass is needed. Be careful on how you connect this kind of elem with the others, otherwise some spurious DOFs may arise... Look in the help file for the appropriate selection of elements and the points you must take care to when connecting different elems types
- from there, "re-grow up" to the translating table where the workpiece is locked, and then to the work-piece itself.
In my opinion, where the workpiece is cut by the milling tool, it should be excitated by the same forces acting "towards the spindle" (the system is "a loop").
You will get automatically this effect without need of duplicate nodes or strange things, if there is a common node between the tool (i.e. it's representative beam) and the workpiece.
- as regards direction of forces: of course you can mill in any direction, but: if your mill-machine is a "portal-type", for example, it is obvious that the machine is less stiff in the direction normal to the portal, so this would be the direction in which to put the excitation vector. There are for sure some guidelines dictated by your own system which only you can know.
- globally, take care in putting elems / real constants which correctly depicts the REAL masses / stiffnesses!!! I know this may sound trivial, but generally it's not so obvious and most of the time some experimental info is needed as regards deflections under known forces.

Well, that's about all, I think...
Feel free to ask there if you still are in doubt...

Regards

 

[krishi1978]

Hi cbrn,

Thanks a lot for your valuable ideas. ANd i am sure it will help me to succeed with my work. Here i have couple of questions. Please try to give me the reply.

1) As you suggested, i can model the machine sturctures with beam and truss elements. But what about the constraints. If i fix them, then i need to consider them as a rigid body. But in this case, what about the vibration absorption in to machine?

2) Otherwise can i take the total machine structure as a lumped mass? Ofcourse here also rigidity would be the problem, i suppose..what is ur idea?

3) here is the new doubt i got yesterday when i was thinking. As i explained earlier i would like to simulate both evenly spaced and differential spaced milling cutter. For the evenly spaced milling cutter, i can apply the load 4* load(4= no.of inserts). When it comes to differential inserts, for example i would like to take 5 inserts with differential pitch. In this case i can`t apply 5*load, since the pitch is not uniform. or it doesn`t matter? So how can i proceed in this case. Could you please give me
some idea?

thanks in advance,
Krishi.

 

[cbrn]

Hi,

1+2) there is no problem as regards restraints: somewhere your machine must be grounded: in real life it is not flying all over the place ;-) ! Internally, let the program make the work for you, by assembling the element matrices (which are stiffness-coeff matrices). If you use a beam, it can bend and resist to compression/traction, for example; if you use a truss, only purely axial load with no bending (the "complicated" equivalent would be to use a beam instead, with two pin-joints at the extremities...), etc... "En passant": there are lots of elem types, of the "COMBINATION" family, which can be useful for creating complicated joints or effects, without talking of the CONTA/TARGET elements, BUT REMEMBER: in HARMIC, no non-linearity is allowed.

3) the answer to this is implicit in something that has been discussed some posts ago: you will have to analyze several load-cases separately, and then combine them by post-processing. This is needed for you not only to superimpose two out-of-phase excitations (i.e., from a post-pro point of view, two out-of-phase responses) but also to account for the constant part of the force (for which you will have to run a static analysis in order to generate the LOAD VECTOR which will be used by HARMIC to give you the "prestressed" response.
I'd suggest to read very carefully the manual as regards load-cases and load-files, as well as loadcases combinations, because it's a bit complicated (at least, it has been so for me) and I fear I could become confusing here...

Regards