Converting part from VMC to HMC looking for advice.

[neurosis]

Our company is about to take what is for this company, a pretty big step. We are hoping to finally purchase a Horizontal Machining Center. Before the owner commits he wants to make sure that our VMC work can be easily converted to a HMC most of which are very simple parts that shouldnt be too difficult or require anything exotic. The job that we are hoping to put on the HMC first is the one that I am about to ask some advice on.

 

We make several configurations of this part. They are all very similar in that the profile is the same on all configuration. The only differences are the height and the step on the ears.

 

The part tolerance is + or - .001 on all dimensions except for the hole locations which are a true position of .0015.

 

Right now we are making this part in several operations due to the inaccuracy of our VMC and we are taking what I consider to be a bad approach to making this part in general. We use double locking vices to machine the profile and basic steps in the part, and separate fixtures to put the holes in and finish the tight tolerance steps on the ears.

 

The thickness of this part ranges from .1 - about .15 on the different floors and again, we only have + or - .001 on the thickness and a flatness callout of .002.

 

I hope to design a fixture that enables us to hold several of these at a time and be able to complete these parts in two operations rather than the four that we are doing it in now. My goal is to be able to use the same fixture to make all of the configurations of this part so that all configurations are only one setup.

 

My question is, can anyone offer any advise on how to hold this part on a HMC. I have kicked a few ideas around in my head but have no experience on an HMC so am hoping that someone can give me a few ideas to play with. I dont expect anyone to design a fixture for me or tell me how to make these parts, but rather am just looking for some advise from people with some HMC experience.

 

The material starts off @ 3 X 6.5 X .5 and is 7075 T7 extruded bar. We also have a configuration of this part that the ears are full and not chopped off that the material is 4 x 6.5 x .5.

 

Here is a picture of the part.

 

[Guest CNC Apps Guy 1]

I'd probably use tabs and precision shoulder screws on a flat plate on a tombstone face. You could probably get 5 parts per tombstone face with a setup like that.

 

As far as changing programs from VMC to HMC, one way Old School MasterCAM planes (Top View/Plane = B0) beats the crap out of New School MasterCAM planes (Front View/Plane = B0) is that all you ever had to do to go from VMC to HMC was change a post.

 

But since you are starting from scratch, I'd recccommend you modify an MD/CD so that your Rotary Axis rotates about Y axis instaed of Z. Then you don't have to ghance anything in your old programs if you want to run them on the HMC.

 

JM2C

[neurosis]

That is kind of what I was thinking, tab it out. The only thing there is to worry about at that point it warpage. These parts seem to like to potato chip. All of the configurations would work well with tabbing except for one.

 

I could come up with a clever way to hold on to the first side (stock) using some kind of low profile pitbull type clamp, again holding on to several parts per face and machine some of the steps and the locating holes in the tabs. I figured at that point I would flip the part over bolting through the locating holes, finish the second side and profile leaving the tabs, and then take a small endmill and machine the tabs down to about .01 and break them off and blend to finish.

 

I wasnt sure if that idea was too far fetched to work. :shrug:

 

As far as programming is concerned, I will be starting completely from scratch, designing all new tooling and all new programs. Probably even mostly different tools than we had used in the past. There was allot of releasing the vice to allow the part to warp, and then machining to finish. We wont have that option now so I think that I will have to plan on taking light cuts with super sharp tools.

[Guest CNC Apps Guy 1]

With 7000 series sometimes I will add an extra op to skin one side first, add the tab holes, then do what needs to be done flipping back and forth. 7000 series does tend to warm more than 6000 series. Yeah, it adds an op, but it's really a nothing op.

[MotorCityMinion]

A whole lot of variables missing here. IMO part quantity is going to dictate the numbers of opps. If an operator can't get parts changed, inspected, deburred or anything else that needs to be addressed before the cycle ends, the spindle sits idle.

 

Sub plates and dowels.

 

Rgh and finish on the same tombstone if possible, that way every cycle spits out finished parts.

 

Stacking the parts may be an option worth exploring.

 

Sounds iffy with only 2 opps, regardless of machine type. From .50 to .15 thick is a lot to take off and maintain dimensional stability.

 

Can the part be clamped on a checking fixture for inspection purposes? Some customers prefer that as it reflects actual usage conditions when assembled and theoretically lowers the cost of the product.

 

I don't know if it's available but I would also consider getting thinner raw material if possible, 1/4 to 3/16, mill it to finished thickness then testing the process capability on a less costly fixture.

 

"With 7000 series sometimes I will add an extra op to skin one side first, add the tab holes, then do what needs to be done flipping back and forth" Ditto that. Sometimes, just breaking the skin on both sides is all it takes to keep things straight.

[mpeterson]

First I would say check into Kurt Vise "Mini-Locks" or Mitee Bite's "Mite Bite" I use them all the time for our fixturing, similar to the Pit Bull but very low profile. Personally I prefer the Mini-Lock, but Mitee Bites are a bit cheaper.

 

Second, sometimes it works out like previous posts you may have to cut the scale off one side before you even start.

 

Another possibility I would say is that we made a cover for an Aerospace company years ago that was Approx. 6" wide by 4" long by 1/2" thick. This thing was all hogged out to .060 thickness with ribs all over it. Well the owner wanted to try to machine it complete and very hard. I was skeptical, it was 7000 series Alum by the way, but we did. Basically this cover came out perfect without any warp-age or twisting.

 

I guess the theory was the harder it was machined it almost stabilized the material. I think we only needed .005" flatness on the back side, but for something so thin, I was impressed, but there where ribs also.

 

Something like this is quite hard to trouble shoot ahead. My opinion is that 7000 series is much more stable than 6000 series, but it may be the difference in parts some of us have made.

 

I wouldn't be nervous about skinning one side, flipping it over, hog it out and rip the back off.

 

Keep in mind the style rake you have on your Face Mill will be a big factor too. Many times using a different style geometry tool makes all the difference for adding stress to a part. Talk to a couple Tooling Reps....a couple!! Not just one..LOL

 

Mike in MN

[neurosis]

This is one job that we are considering dedicating 1 face on two tombstones to and never tear down unless necessary. We run quite a few of these and it is a job that would be worth leaving set up.

 

I would like to run both sides of the part on each face of both tomb stones. So we will have complete parts coming off of the machine. That way we can monitor anything that may become an issue.

 

quote:

---

Stacking the parts may be an option worth exploring.

---

Not sure what you mean here.

 

quote:

---

Can the part be clamped on a checking fixture for inspection purposes? Some customers prefer that as it reflects actual usage conditions when assembled and theoretically lowers the cost of the product.

---

Unfortunately not.

 

quote:

---

I don't know if it's available but I would also consider getting thinner raw material if possible, 1/4 to 3/16, mill it to finished thickness then testing the process capability on a less costly fixture.

---

It takes .5 material to get a complete part. Although all of the thicknesses range from .1 - .15, the total thickness of the part at its thickest point ranges from .38 - .425 or so.

 

quote:

---

"With 7000 series sometimes I will add an extra op to skin one side first, add the tab holes, then do what needs to be done flipping back and forth" Ditto that. Sometimes, just breaking the skin on both sides is all it takes to keep things straight.

---

This is definitely something that we are considering. We may just do a skinning operation on a separate machine. It would probably be well worth the time. In fact, we skin one side of the parts now prior to roughing out the first side.

 

 

quote:

---

First I would say check into Kurt Vise "Mini-Locks" or Mitee Bite's "Mite Bite" I use them all the time for our fixturing, similar to the Pit Bull but very low profile. Personally I prefer the Mini-Lock, but Mitee Bites are a bit cheaper.

---

We use Mite Bite clamps quite a bit. I think that the pitbull clamps are a mite bite product arent they? They have several low profile clamps that we are thinking about trying. I am even thinking about building some dove tail fixtures using their machinable clamps.

 

quote:

---

Keep in mind the style rake you have on your Face Mill will be a big factor too. Many times using a different style geometry tool makes all the difference for adding stress to a part. Talk to a couple Tooling Reps....a couple!! Not just one..LOL

---

I will be looking in to this for sure. Ive experienced how the wrong tool can put a butt load of stress in to the material. Even something as simple as a chipped insert can take a perfectly good running part and warp the hell out of it. Now that we will have a very good machine it will be worth buying the best tooling for it. Once we get it, the pressure will be on me to make sure that we are able to make money with it. I am the one that has been pushing to get a horizontal.

[Justin Beebe at Folsom Tool]

To me that part looks like it could be completed in one operation on a horizontal mill if you hold it in a window frame. It may be hard to hold the thickness of +-.001

[MotorCityMinion]

I didn't realize that they were .38 to .425 thick. The stacking was in reference to the .10 to .15 thickness. 6 to 8 pieces stacked together, drilled thru in non critical holes, screwed down, clamps moved, then continue machining.

[neurosis]

quote:

---

To me that part looks like it could be completed in one operation on a horizontal mill if you hold it in a window frame. It may be hard to hold the thickness of +-.001

---

Ive heard of machining parts this way but have never seen it. Ive heard that it works very well for some things. I may have to try to dig up some examples of this.

[Mic6]

What machine is it and what options did you get?

[neurosis]

Not to get off subject here , but we havent committed to any machine at this point. I know which machine the owner is leaning toward for sure though. I wont say until its a done deal as he still isnt convinced 100% that we have the right work to make it worth it. His decision hinges on whether or not we can come up with some good ideas on how to tool some of these jobs for the horizontal. He wants to make a definite decision by the end of this month so its crunch time.

 

This part that I am talking about in this thread is one of the two jobs that I am having the hardest time figuring out a good way to tool them that will be both simple and efficient. If I can come up with a fast and effective way to tool this job, and one other on a Horizontal, then he will be sold.

[Nick Eaton]

You might also consider using plate rather than extrusion.

The extrusion process tends to concentrate impurities and inperfections in the outer skin, so when you remove it assymetric forces "warp" the material.

Skinning the part first mitigates this problem.

Substituting plate can allow you to skip the skinning op as the material is more "stable" and consistant.

Keep your chipload as high as you can to get as much heat in the chip as you can,

Nick Eaton

[Mr. Wizzard]

I'm not sure what your profile tolerances are, but I have a suggestion.

 

What about water-jetting the profile from plate, then making fixturing with the profile milled into it however deep you need.

 

Part fits in like a cookie-cutter. Then bolt thru your through holes and go.

 

I have done many thin part this way, but it depends on your profile tolerance and finish requirements.

[Colin Gilchrist]

Hi Dave,

 

I'm with Nick on this one. I'd go with a large plate that get's bolted into a window frame tombstone (think large "T" style plate with a square hole cut in the center). The plate could be held on the edges with cam lock clamps.

 

Because the Tomb is basically a large rectangular window, you can machine both sides of the part by just rotating the B axis 180°.

 

You could nest 6-10 parts into the plate depending on your machine.

 

Start by skinning one side of the plate, rotate the tomb, skin the second side, then machine all your steps and other (non-hole) features.

 

Rotate back to the first side, finish the steps on this side, then machine all your critical holes.

 

The final step would be to profile each part leaving material tabs that hold each part to the frame.

 

The advantages of doing it this way are many:

 

1. Only one clamping of the material.

2. Only one fixture required (the excess material acts as the rest of the fixturing).

3. Easy setup: the only thing you have to get perfect is the work offset to the centerline of the pallet rotation.

4. Modular: One fixture and you can do the entire family of parts (or any other part you can fit in a plate of similar size).

[neurosis]

Do you guys have or know of any photo's of examples of parts being run in a window frame as you are suggesting?

 

I wonder how flimsy the parts are going to be once you get everything roughed down close to the finish thickness? This sounds like a very easy set up for sure but I have 0 experience running parts with a window frame type setup.

[Justin Beebe at Folsom Tool]

Neurosis,

 

I have done hundreds of parts in window frames. The parts will not get flimsy at all if this type of machining is done correctly. One more advantage of machining this way is that all the clamping force is away from the area you are machining so the parts stay very flat. I can't share our files but I can try help you out if you have any questions.

[Colin Gilchrist]

Dave,

 

If you spring for the beer, we can sit down for a few hours and I'll show you some examples. You would be amazed at how strong a .01-.02 tab can be. I've got a few examples (pre-Boeing work that I've done), but nothing I can post up here.

 

You will love it and so will the owner, this I promise.

[neurosis]

Colin,

 

Let me know when you have some free time and what kind of beer you like to drink. That sounds like one hell of a deal to me.

[Jayson Kramer]

Neurosis you will find this to be a useful tool for allot of parts. Also you should have a good time with Colin, he is good people.

 

It's good to hear that allot of you are using this. you would be surprised how many people look at me like what is window frame machining.

[MotorCityMinion]

Sounds like you may be able to tool up sides of the window frame fixture to remove the tabs also. If need be, the top can also be tooled up.

[MotorCityMinion]

Large, single part fixture:

 

 

[neurosis]

This is all great advise. I may talk to the boss and see what he thinks about it. If I can get a meeting set up with Colin I may try to go over some ideas and ask a few questions about my concerns with this particular part.

 

quote:

---

Neurosis you will find this to be a useful tool for allot of parts. Also you should have a good time with Colin, he is good people.

It's good to hear that allot of you are using this. you would be surprised how many people look at me like what is window frame machining.

---

Ive spent a few hours with Colin when I first started using Mastercam. In hind sight, I wish that I would have waited about two more months before meeting up with him. I would have had some better questions for him if I had. I appreciated the time that he spent with me. Very cool guy and very easy to talk to.

[1 master]

he does seem to be a cool guy. Make me wish i was still in seattle. Help from him is better than school.

[Colin Gilchrist]

Hi Dave,

 

Fridays are good for me, I work M-Th. Are you free tomorrow afternoon/evening? Saturday I'm pretty slammed, I'm helping a buddy with an engine build and install.

 

If this week won't work on such short notice, maybe next Friday/Sat?