Cylindrical Grinding Before Surface Grinding?

Welcome to the forum. And hopefully you will continue with us and not be one of those one time visitors.

It is difficult for us to comment. We do not have any idea of the shape of the component.

It will be helpful if you just enclose a brief sketch

(You can have a jpg file created through scan/ CAD or any other method) and attach here by pressing the camera button above this frame.)

This will ensure there is no miscommunication.

In our case - We too do the faces first (ours are generally shafts) - create the centers then the lathe and cyl grinding operations both are done between centers.

If you do the cyl grinding first- the diameter will be mede first - likely between centers ?. I can assume this will not be likely perpendicular to the face.

Later when you grid the face how are you going to maintain the perpendicularity of already finished dia with the faces ? The setting of the job itself will be problem. It is not only putting packings here and there but also how to ensure the diameter ? dialing along axis in a circular profile is very complicated and unless extreme care is taken is error prone.

However a flat face can always be dialed along periphery as well as radially to ensure the correct setting.

This is assuming the perpendicularity is critical.

If it is not, it doesn't matter which operation you are doing first.

You can do it and you do it after. Because the process of surface grinding you are doing is not exactly with ref to centers.

You can use V Blocks Or some fixtures for this purpose

what if you centers are like this picture?They are not Going to offer you perpendicularity anyway.

I think I understand what you are trying to do. I do a similar procedure when I have to surface grind vacuum pump stators. If you don't surface grind first you will have no way of knowing whether your perpendicular end to end. As long as your perpendicular end to end than your cylindrical bore will be straight otherwise your eye will have no good frame of reference to judge whether or not your going to end up with a straight bore. As long as your square end to end it should work.

But the question is How are you going to make sure that both the centers are parallel to outer cylinder and also perpendicular to faces?if not perpendicularity of faces will be lost after cylindrical grinding anyway.

Refer #1 - Job setting on grinding (even if no center on job) can be done (and are done through clamp plates having centers. When you do cyl grinding, the jobs are dialed through these clamp plates fixtures (borth radially) and peripherally on one face.

This is easily done on the face which is a plane surface. However if I do otherway, dialing across axs, and re-setting is just a bit too difficult and error prone.

Obviously not.

If the two faces are not parallel, you will end up with a tapperd shape, not a proper cylinder. Surface grinding the ends will not fix this problem.

the idea of surface grinding the ends first, is to make sure that the centerline of the work is concentric with machine's axis so that you can get a proper cylinder.

I am sorry, but this practice is being done, with fixtures in components where the faces are not required to be ground (turning finish is good enough) but the end details for dead/live centers can not be done.

And unfortunately no taper are at least measurable.

Thanks for your reply.

Above is the drawing I need to finish. Usually I grind the datum B (roughing), then I grind the opposite face to make it parallel (surface grind). After that process, I move to the cylindrical grinding to grind datum A, I dial the surface datum B. Then I finish all cylindrical dimension. So I can reach all tolerance.

If I change the process, first I grind datum A (cylindrical) and finish all cylindrical dimension, then I finish datum B and thickness 20 in surface grinding, can I still get the perpendicular between datum A and B?

The drawing shows that you are going to hold the job in a taper mandrel for doing the cylindrical grinding.

One thing is sure here that you will not be able to dial the diameters effectively too get the tolerances within spec The length of the cylindrical portion is only 15mm.

Hence by your new process you are going to need an indirect method of measurement that has to be accurate enough to override the measurement inaccuracies.

I assume that the bore is finished in turning ? or you are reaming/ honing it while grinding B. In that case I don't see a job holding point.

Look at the process how are you maintaining the perpendicularity between the ground face B and the bore.

So the possible processes as I can see is

1) Rough turn all dims and finish turn the bore.

2) Grind the face B

3) reverese and grind the opposite face

4) Fix a mandrel in the bore.

5) Hold the mandrel bet centers in the cyl grinding, dial the face B and grind the dia A

In this case you have already lost the perpendicularity between B and A.

In other variant

in 1) Leave a total length allowance (for holding the job) and allowance in bore.

4) Dial the face B and holding the job on chuck, finish bore A (turn'grind'hone)

5) Grind the face opposite to B to finish size.

6) and 7) similar to last 2 steps. (4) and (5)

With the accuracies required, I always prefer the existing technology.

However what I can think about is

a) Gold on the opposite of B, finish the A, and B. You have face grinders that can be accommodated on lathe and the bore can be done to your requirement on the lathe itself (using the tailstock as tool holder if needed).

b) Part to length. and carry out the cylindrical grinding (ie if you can not do that too in step-1)

c) Now face, grind, whatever you want to do with the opposite face on surface/segmental grinder.

In this way in one undisturbed setting you are generating the OD, B and A.

It depends on your facility and tooling. (also there are tools available if you don't want to do the cyl grinding itself) - diamond polishing bits etc,

I forget to add other information.

The material is Carbide ( pre-formed 0.5mm /side).

(All my lecture goes down the drain.. at least vermatim)

0.5mm per side means case carburised isn't it ?

Of course you still have hardcutting tools (check web) able to cut greater then 60HRC but never had to resort to in my work area. Here we always go ahead with grinding in case of hardened components.

Of course the other portion still works (and likely to work) is the usage of grinding attachments on lathe.

All the surfaces are carburized or only the A and B ? How are you machining the bore ?

It is possible to modify what I can imagine , and you can see that it is not mandatory to grind before.

BTW we always as manufactureres try to finish critical, reference and dimensions having geo,metric relationship in minimum number of settings - you know whatever may be your accuracy of setting/dial gauge, the errors in each step stack-up they may as well add up rather than cancelling each other - cancelling is only at zero degrees all other 360 degressa cause addition (vector)

Look from this angle, and look for hardcutting tools, rolls etc to get you the finish on lathe.

It's not carburized, the material is tungsten carbide, hard metal product submitted to sinter-hip heat treatment, mainly used for cutting tools, ie insert for turning.

So, I always proceed them in grinding mch, with diamond tools.