[philbur]

Hi Dennis, I don't understand your point. A chip load of 0.001" per rev at 18,000 rpm is only 18 ipm. Do you consider this as an accessive feed rate? At 5,000 rpm it's only 5 ipm. That's on a par with watching grass grow.

With a fine tip a chip load of 0.001" per rev might be a bit high, so to keep the feed rate up you need even higher rpms on the spindle!

I'm not sure what you mean by a feed rate of 100 fpm. Is that feet per minute?

I've never come accross a commercial cnc engraver with a 5,000 max rpm spindle speed.

Maybe I'm missing something!

Phil

You really do not need a faster speed in that the tip of the engraving tool is so small that with a chip load of 0.001 inches per rev the feed rate would have to be tremendous to keep up with an 18,000 rpm spindle ( I have one of those also). Because of acceleration factors, there is no way that a milling machine can use high speed spindles to full advantage in engraving. You can program your feedrate to be 100 fpm, but in reality, with a bunch of tiny cuts and lots of ups and downs you will be lucky to achieve 1/10 of that.
Dennis

[Sp-4renegade]

dumb question. the chip load .001 that would be per tooth 4 teeth 72 inch per min. Or am I wrong?

[Rendrog18]

dumb question. the chip load .001 that would be per tooth 4 teeth 72 inch per min. Or am I wrong?

arent most engravers only 1 tooth? or is this a dumb question?

[philbur]

Here's a typical engraving cutter.



Phil

[Dennis Rech]

Hi Dennis, I don't understand your point. A chip load of 0.001" per rev at 18,000 rpm is only 18 ipm. Do you consider this as an accessive feed rate? At 5,000 rpm it's only 5 ipm. That's on a par with watching grass grow.

With a fine tip a chip load of 0.001" per rev might be a bit high, so to keep the feed rate up you need even higher rpms on the spindle!
I'm not sure what you mean by a feed rate of 100 fpm. Is that feet per minute?
I've never come accross a commercial cnc engraver with a 5,000 max rpm spindle speed.

Maybe I'm missing something!

Phil

Hi Phil.
There is a typo. The rep at Onsrud recommended a chip load of 0.004 per revolution so this would be 72 inches per minute feed rate. At 6000 rpm the feed rate would be 24 inches per minute. If you are using a cutter with two surfaces you need to double this.
I have a 30,000 rpm secondary spindle attached to my mill and also a ShopBot that has an 18,000 rpm spindle. I use them all. I called Onsrud to find out why all the engravings had the same problem and what the correct feeds and speeds should be.
He explained that mills with their heavy moving masses cannot accelerate nearly fast enough to provide the theoretical feeds even with large servo motors. I watched mine while engraving. He is right. My engravings consist of text that has thousands of little lines. Each requires a start, stop, rise and plunge. So even though I have a mill capable of very fast rapids, the machine cannot attain those speeds in 1/32 inch bursts.
Onsrud recommended to me a spindle of 4500 to 8000 rpm max with 20 to 24 inches per minute as a realistic feed rate with attention paid to chip removal.
It works well for me.
The commercial engraving machines that I have seen can have high speed spindles but light moving masses. They probably can accelerate quicker than a milling machine.
They usually are engraving plastic trophies and plaques and need those feed rates to prevent the plastic from melting at high rpm.
My best engraving in 6061 t6 aluminum 0.022 inches deep are at 4500 rpm with a feed rate of 22 ipm with lots of coolant and air.
The gist of the story is that a Tormach 1100 should be able to engrave just fine.
Dennis

[philbur]

.004" per rev is one hell of a feed for a fine tipped engraving cutter. For a 0.008" tip it would be greater than the clearance, meaning that you would be forcing the back side of the cutter through the workpiece and risk breaking the tip. The chip load per rev must be a function of the cutter tip width. A chip load per rev of 10% of the cutter tip width is a good starting point I think.

In a previous thread in January you did say, and I agree:

For engraving plastic, aluminum and even steel, I prefer the router with the much faster spindle (a secondary high speed spindle can be piggybacked on the mill).

Phil

[Dennis Rech]

.004" per rev is one hell of a feed for a fine tipped engraving cutter. For a 0.008" tip it would be greater than the clearance, meaning that you would be forcing the back side of the cutter through the workpiece and risk breaking the tip. The chip load per rev must be a function of the cutter tip width. A chip load per rev of 10% of the cutter tip width is a good starting point I think.

In a previous thread in January you did say, and I agree:

For engraving plastic, aluminum and even steel, I prefer the router with the much faster spindle (a secondary high speed spindle can be piggybacked on the mill).

Phil

I pulled out my notes from the conversation with Onsrud. I told them 6061 T6 and 0.022 depth. They suggested 0.004 as a chipload. With a 60 degree angle and 0.010 tip, the engraving should be about 0.035 inches at the top which is what counts to me. I just measured the line widths with my good micrometers. The actual width is between 0.029 and 0.041. So depending on whether chip load is measured at the top or the bottom of an engraving cutter, 10% or 0.004 may be fine. Let's call it 0.001 at the tip and 0.004 at the top.
All this is moot, however. My engravings are all text, between 1/8 and 1/4 inch high. The longest pass in it is 1/4 inch. So, for each letter, my engraving tip plunges down 0.022 inches and is at a zero feed rate. The 400 pound table then accelerates 1/8 inch trying to get to 22 IPM, then decelerates 1/8 inches back to zero.
So what is the feed rate? Right after the plunge, it is 0 divided by 6000. If the cutter is rotating 18,000 rpm its 0 divided by 18,000. It then climbs to something as the table accelerates for 1/8 inch. Then it works its way to zero again. There is a lot of energy going into chips that are not carrying away much heat. That is why the chips were welding themselves back into the engraving in my case.
The solution was to energetically blow them or wash them away.

Previously, while engraving with the ShopBot ( no coolant), I found that higher rpm worked better in that it threw the chips up enough that the vacuum system could carry more of them away before they re-welded themselves to the material.

So back to Umesh's original question of can a Tormach 1100 be used for engraving. I still say yes as long as the coolant keeps spraying.
Dennis

[Sp-4renegade]

Thanks Phil, I learned something, nice pic of tool.

[philbur]

Of course you can engrave with a PCNC1100, it's just not the right tool for the job if your main target is engraving.

Note that the OP didn't ask: "can the PCNC1100 be used for engraving" he said "I need 1 CNC engraving machine, which machine should I purchase".

The PCNC spindle speed is to low for a dedicated engraving machine. Tormach do provide a strap-on high speed spindle and a speed increaser, both of which are compromises if your main goal is engraving. If he needs an engraving machine he should buy an engraving machine, not a milling machine.

As the weak point in an engraving cutter is the tip I think it is wise to relate the chip load to the tip not the top end of the cutting edge. If the rate of advance of the cutter is greater than the cutter clearance/relief at the tip, you will be partially drag engraving, which is not necessarily a problem in soft materials but does put the tip of your expensive carbide cutter at risk in harder materials like steel.

Phil

[philbur]

If you look at the diagram you can see that the cutter can advance by a distance equal to the clearance value in half a revolution, before it will start to rub. So to my mind the maximum safe chip load is 2 times the clearance value per rev.

Just a thought

Phil

[Dennis Rech]

Of course you can engrave with a PCNC1100, it's just not the right tool for the job if your main target is engraving.

Note that the OP didn't ask: "can the PCNC1100 be used for engraving" he said "I need 1 CNC engraving machine, which machine should I purchase".

The PCNC spindle speed is to low for a dedicated engraving machine. Tormach do provide a strap-on high speed spindle and a speed increaser, both of which are compromises if your main goal is engraving. If he needs an engraving machine he should buy an engraving machine, not a milling machine.

As the weak point in an engraving cutter is the tip I think it is wise to relate the chip load to the tip not the top end of the cutting edge. If the rate of advance of the cutter is greater than the cutter clearance/relief at the tip, you will be partially drag engraving, which is not necessarily a problem in soft materials but does put the tip of your expensive carbide cutter at risk in harder materials like steel.

Phil

Hello again, Phil
I agree that an engraving machine is the proper device to use if one is engraving. Unless the part to be engraved is 4 feet long and weighs 60 pounds. Then the engraving shop tell the customer to find someone with a bed mill.
It just happens that I am an acquaintance of the gentleman from India that ask about the Tormach although I have not chatted with him for awhile. He is building one of my telescope mirror fabricating machines. I'm guessing that he needs a milling machine that can also do some engraving. I sent him an e-mail to see if he needs anything specific and am looking forward to hearing from him again.
I'll also agree that an actual chip load of 0.001 may be about right for a flat engraving bit as long as one keeps in mind that with a mill, you can calculate a lot higher chip load and acceleration factors will greatly lower it.

This morning, I ran a fixture of engraved plates. Each was 2x14 inches and if I had measured the length of each text segment and the distance between segments and the distance up and down, the total length of all the movements together was probably 48 inches. At 24 inches per minute, each plate should have taken 2 minutes. In reality, it takes 16. My actual feed rate was 3 inches per minute and at 4500 rpm the chip load was more like 0.00067. Looks like the spindle can be slowed a bit more, but I am getting excellent engraving now and won't mess with it.

The problem that I had when running the high speed spindle at 18,000 rpm was burnishing. The melted aluminum looked a bit smeared and the aluminum chips (more like fine filings) embedded themselves into the melted aluminum. The text was a bit ragged. At 18,000 RPM my actual chip load would have been 0.00016.

The 12,000 rpm ShopBot has the same problem unless I put an air blast right at the cutter tip to remove filings. It still burnishes and the tip gets edge build up without coolant. The ShopBot also has a problem with text under 1/4 inch. Probably too much backlash in all three directions.

Onsrud does not recommend their engraving bits for steel. I have even chipped the tip off in extruded acrylic plastic when the plunge rate was a bit too high.

Just out of curiosity, has anyone on this group used their Tormach for engraving? What have the results been?

Dennis

[philbur]

Here's some steel engraving I did a few years ago on my PCNC 1100:



From memory: 4200 rpm - 100 mm per minute - 60 degree cutter. Text size is 3mm.



Phil

Just out of curiosity, has anyone on this group used their Tormach for engraving? What have the results been?

Dennis

[philbur]

Hi Dennis, OK I understand your point about higher feed may not gain much increase in speed when moves are small. However I just did a test on my PCNC 1100.

I simulated a 20 pass engraving of the figure 8 as a single line text 3mm high.

First run with F = 100mm per minute took 1 minute 59 seconds.

Second run with F = 500mm per minute took 24 seconds.

5 times the feed rate gives 4.96 times less milling time.

a 500% increase in spindle speed from 5,000 to 25,000 would give me a 496% reduction in milling time while maintaining the same chip load per rev. There seems to be no measurable limitation imposed by the maximum accel/decel rate.

Agreed that at the higher rate coolant may be necessary.

Phil

[UmeshG]

Hello,
My Name Umesh
I am From India (MUMBAI )

Any Body Use Tormach 1100 For Engravng Porpes ?
Please give me feed back.
I am Engraver . I do Small Engraving , Melediyan dies , Numbring Punches , Stamp Marks, Many Types Of 2D & 3D Engraving Jobs. I Need Multy Perpose Machine For Engraving 4Axis & Small machining Part .

Can I Purches PCNC 1100 Serise3 Machine.
Please Give Me feedback About Tormach PCNC1100

Thanking You

[philbur]

Hi Umesh, I have done engraving with a Tormach PCNC1100 it works fine but is slow, especially if you intend to do it on a commercial basis. A PCNC 770 with a spindle speed of 10,000 rpm will almost certainly be a better choice for your needs.

Phil

Hello,
My Name Umesh
I am From India (MUMBAI )

Any Body Use Tormach 1100 For Engravng Porpes ?
Please give me feed back.
I am Engraver . I do Small Engraving , Melediyan dies , Numbring Punches , Stamp Marks, Many Types Of 2D & 3D Engraving Jobs. I Need Multy Perpose Machine For Engraving 4Axis & Small machining Part .

Can I Purches PCNC 1100 Serise3 Machine.
Please Give Me feedback About Tormach PCNC1100

Thanking You

[UmeshG]

Hello,
My Name Umesh
I am From India (MUMBAI )

Any Body Use Tormach 1100 For Engravng Porpes ?
Please give me feed back.
I am Engraver . I do Small Engraving , Melediyan dies , Numbring Punches , Stamp Marks, Many Types Of 2D & 3D Engraving Jobs. I Need Multy Perpose Machine For Engraving 4Axis & Small machining Part .

Can I Purches PCNC 1100 Serise3 Machine.
Please Give Me feedback About Tormach PCNC1100

Thanking You

[MichaelHenry]

QUOTE=Dennis Rech;1103115]Hello again, Phil
Just out of curiosity, has anyone on this group used their Tormach for engraving? What have the results been?Dennis[/QUOTE]

I engraved acrylic early in the life of my Tormach with the results shown here:



AIR, the auxiliary spindle (die grinder) was used with a bit from Bits & Bits that was held in a collet. It all seemed to work pretty well, although a spring-loaded holder would have worked better. Those aren't available for the die grinder spindles so far as I know,