tip comp

[Hugh.Venables]

On the surface parameters page it is possible to toggle between tip and centre for tip comp. It doesn't seem to make any difference. Surely it should to, say, a ball nosed cutter?

Thanks, Hugh.

[Guest CNC Apps Guy 1]

The difference would be when you touch off your tool. You need to add(or is it subtract?) the radius of the tip or else you'll be too deep.

 

You shoudl see a visual difference in the toolpath if you have enough radius on the tool.

 

JM2C

[Hugh.Venables]

Thanks James. I'm machining a small aerofoil (25 m.m. x 3 m.m. x 200 m.m. long) with a 20 m.m. ballnose tool. Around the front it machines around 90 degrees, (How do you get a degree symbol from a keyboard?) at least it does when I write the last few lines down to the centre line. It doesn't seem to matter whether tip comp is tip or centre. Maybe it only affects the tool touch off, as you said.

Thanks, Hugh Venables.

[Finecut]

Hugh

The deg symbol is : ALT + 0176 on the keypad

Hold down the ALT key and type in on the keypad

0176

 

Finecut

[cadcam]

Vary cool fine cut never new that.

Another key trick for me.

[Rick Damiani]

quote:

---

Thanks James. I'm machining a small aerofoil (25 m.m. x 3 m.m. x 200 m.m. long) with a 20 m.m. ballnose tool. Around the front it machines around 90 degrees, (How do you get a degree symbol from a keyboard?) at least it does when I write the last few lines down to the centre line. It doesn't seem to matter whether tip comp is tip or centre. Maybe it only affects the tool touch off, as you said.

---

When you say you are seeing no difference, is that in MasterCAM's verify, the toolpaths that MaterCAM displays, or in the parts you are making? Verify won't show a difference, nor is it easy to see the difference in backplot unless you are looking for it. It will make a big difference in the part though.

[Hugh.Venables]

Finecut, thanks very much for that. I've been trying to find out how to do that for years. Got a new problem, though. Got to figure out how to remember it............

 

Rick, please tell me more. Can you expand on the sort of difference it will make. I used "tip" without thinking as it's the default. The part looks good but is difficult to check. Might be able to look at the end of it in the profile projector using surface lighting. Can't find anything in help that explains tip comp any further. Just had a look through the V8 Applications guide. Couldn't find any information or any example where "center" was used.

 

Hugh Venables

[Guest CNC Apps Guy 1]

I've almost always used Tip. The times I've changed to center was when I was cutting Vertical Walls. It seemed to comp better in those situations. You must however touch your tool off differently that when Tip is selected. As I said earler you must add the corner radius value to the length (or subtract the corner radius value depending on which way you look at it).

 

BTW, you'll not see any differences in Verify. You'll see differences in Backplot only if you know what you're looking for.

 

Hope that helps.

[cadcam]

I use to use center of tool years agao when we did not have tip of tool. this was like V3 & V4.

 

And I am like james and have used it on a few other ocasions (SP?) over the last years.

 

[ 08-04-2002, 08:16 PM: Message edited by: cadcam ]

[Hugh.Venables]

Thanks James. Thanks Jay. I guess what I'm most concerned to find out is whether the part will be produced accurately using either method. Rick's reply suggests a possibility that it may not. James, your reply suggests that too. What differences am I looking for in backplot?

Hugh Venables

[BernieT]

quote:

---

...is whether the part will be produced accurately using either method. Rick's reply suggests a possibility that it may not. James, your reply suggests that too. What differences am I looking for in backplot?

---

Hugh, either method will produce an accurate part. Like said before, the difference is in the touch-off. In 'backplot' look for the the toolpath at the tip of the ball tool or at the center of the ball tool. (With a flat end mill you wont see any difference) The possibility of error occurs if you set comp to 'center' and touch off to 'tip' or vice-versa without adjusting for the cutter radius.

 

BerTau

 

[ 08-04-2002, 10:21 PM: Message edited by: BerTau ]

[cadcam]

The only difference occurs if you do not touch the tool off correctly.

Other wise it will cut the surface the same.

 

So good luck if you should decide to take the job.

These boards will self destruct in 100 years so please backup.

[Hugh.Venables]

Gentlemen, thank you all for your input. I'm not just relieved, I'm better informed as well.

Hugh Venables.

[Rick Damiani]

quote:

---

Rick, please tell me more. Can you expand on the sort of difference it will make. I used "tip" without thinking as it's the default. The part looks good but is difficult to check.

---

Either compinsation method will work so long as you make the appropriate adjustments when you touch off the tool. OTOH, if you were to use 'center' and not add the tool radius to the Z value when you touch off, your part will off in Z by the tool nose radius. For flat end mills (which have a tool nose radius of 0.00) there is no difference, of course.

 

Verify assumes that the tool was touched off correctly, and so will not show a diference. In backplot you can see the diffeence by looking at where your toolpaths lie in relation to the surface in question. With center compinsaiton and a ball or bullnose endmill, the path will be above the surface. With tip compinsation, it will be right on the surface.

 

It is important to note that tip vs. center compinsation will not produce the same toolpaths if you are programming a two- or three-axis move that invovles a complex curve. Take a look at fig. 7.38 on this page:

 

Big Book for Windows ch 7

 

MasterCAM tries to keep the surface tangent to the radius of the tool nose, and so has to follow a different path for center vs tip comp.

[cadcam]

So rick you are saying in the case of multi surface it will cut it diffrent or in the case of a steep transtion between 2 surface it will be diffrent.

 

I am trying to see were it will go wrong from what you are saying.

This tool to center is all we use to have and I was able to make molds correctly useing this path when we checked the Die it was right..

 

I do know that the code and the way mastercam looks at the path will be diffrent.

 

Thanks for your time rick.

 

how was your trip?

 

[ 08-05-2002, 10:12 AM: Message edited by: cadcam ]

[Hugh.Venables]

Jay, Rick is just saying the toolpath will be different for tip or centre compensation. I don't think he means to imply that the machined part will be different.

Rick, what is that Big Book?

Thanks again guys, Hugh Venables.

 

[ 08-05-2002, 07:31 PM: Message edited by: Hugh.Venables ]

[Rick Damiani]

Jay wrote:

 

quote:

---

So rick you are saying in the case of multi surface it will cut it diffrent or in the case of a steep transtion between 2 surface it will be diffrent.

---

The path itself will be different, and the difference will depend on the cutter geometry. The part will come out just the same, provided you adjust the tool offset correctly.

 

As for my trip: The certification class I was supposed to attend got cancled, dag nabit. I did spend the week before last near Boston though, and that went well.

 

As soon as we get a schedule for the next round of classes I'm gonna get to go to them.

[Rick Damiani]

quote:

---

Rick, what is that Big Book?

---

The Big Book for MasterCAM is a very large textbook written for MasterCAM V7 and updated (somewhat) for V8. It's kinda pricy and getting kinda hard to find, but it contains much useful information.

 

The link I posted takes you to an HTML version of ch 7 of that book. Follow the URL up and you can get to a PDF version and/or the rest of ch 7 and the first chapters, which takes you through basic 2D paths and associativity. The rest of the book is toolpath planning and 3D toolpaths/geometry. Very useful book.

[cadcam]

Rick did you see the Rock? (Plymouth)

Also how is Mike Frimann (Sp?) doing?

 

Well welcome back ready for class again?

 

J

 

[ 08-05-2002, 10:38 PM: Message edited by: cadcam ]

[sir Camalot]

Rick,

I just wanted to say thanks for the link! Pretty cool info. I think this would be a good start for a resource information page or folder.

Maybe the forum could start an educational resource and or links page that would allow users to offer and use this type of information for easier access. This might could include shareware related to Cam and machining, educational sites, tooling-- anybody have some other ideas? We all know of a few sites, maybe if we all shared we could develope a huge resource list.

Thanks again!

[cadcam]

sir Camalot I like this idea.

I would like this info so I may put a page on my web site with this info that all of you may go to and I will keep it updated as more come in.

 

Then the webmaster could link to it as a refrence to links page.

 

Any thoughts on this?

 

J