custom designed tools

[JAMES GABEL]

I am trying to setup a library for my tool holders and tools. I sketched out all my holders and drew one of my cutters in with one. I want to be able to pick that custom tool file and use it to back plot and verify. When I make my tool path I use the user defined, that works great in back plot but in verify it shows the wrong form on the end of the cutter. I did chose user-defined on verify and that did not work. That makes me uncomfortable. I also tried choosing a ball end mill and pick custom file and that made the tool 1/4 the size it was before.

[JAMES GABEL]

Bump

[JAMES GABEL]

I drew up a ball em and in verify it shows a cutter with an angle to point like a chamfering tool. I have been drawing up the cutter and holders just like you said and it comes in verify with a different tip on the cutter.

[JAMES GABEL]

If I go to tool type tab and pick a ball em and then pick a custom tool profile the tool shows 1/4 the size in back plot and verify. If is use the undifined tool it looks good in back plot but not in verify. I am confused. I know this is a very simple thing but I am drawing a blank on what to do.

[DavidB]

quote:

---

If I go to tool type tab and pick a ball em and then pick a custom tool profile

---

James

If you defining a CUSTOM tool use the UNDEFINED Tool type.

Dont define a custom tool and select a standard tool type (Sper Mill).

 

HTH

[Matthew Hajicek - Singularity]

I always use the flat endmill tool type and draw at a 1" radius. It works perfectly, but the scaling is annoying. I'll have to try drawing the tool to size and using the undefined tool type. It would appear that both ways work.

[Paul Felger]

Hey guys, I am using XLathe, and while on the subject I use kennamet tool library the most and use a lot of custom ground c2 tools in the machine. Is there a way on lathe to draw up my own tools insted of modifying the inserts and holders? We do a lot of face and small id work.

 

Thanks,Paul

[Guest John Paris @ Services 4 Automati]

Paul,

 

If I can make a suggestion, it sounds like you could really use a training class.

 

You should probably call your reseller and get one or two scheduled. They would go a long way to helping you understand and solve your issues.

[DavidB]

Paul

In Lathe draw the tool in color 14 and the holder in 116

 

In MC help look at "Tool definition"

[Paul Felger]

Thanks John,

 

I have taken classes and it was all out of box tooling in the class. That is what I am use too, but this is a new job and they use custom tooling. Dont think I need a class when someone like you could answer my question. Yes or No can you custom draw your tools on X lathe?

[Paul Felger]

Thanks Dave,

 

You gave me the right answer Dave, Thanks

 

We do some crazy undercuts and face profiles, out of the box cant produce.

[JAMES GABEL]

In verify it does not allow me to chose full radius. It only allows me to pick angle and corner. If I pick corner and give it the rad. It is still wrong.

[DavidB]

Email me your file

[DavidB]

James

Just change the tool tolerance to .003 in the verify config, and turn the Speed/Quality slider all the way to Quality.

 

HTH

[JAMES GABEL]

Thank you very much. I can't believe it was that easy. I feel real smart right now. I appreciate your help very much, you saved me a lot of headaches.

[DavidB]

Glad I could help

[kunfuzed]

I'm trying to get a realistic representation of a center drill. I think I'll need a file for each size. Problem is it works fine when I use "Custom Level", but in "Custom File" none of the fields adjust any of the tool lengthes. Any Ideas?

[Guest CNC Apps Guy 1]

You need to make it an "Undefined" Type an d just use the Level or File and use the first diameter as the tip diameter and set the shank diameter correctly as well.

 

HTH

[kunfuzed]

I'll try that. Thanks!

[Racerje]

Just wanna say thanks I have been struggling with creating new tools for like a month never tried to use undefined works great now many thanks to all the great people here I try to read the forums everyday and I usually learn some thing new everyday!!

[Guest CNC Apps Guy 1]

You're welcome!

[JAMES GABEL]

Back on this subject again, I just started running a job and I am using a defined tool on a tool path. I am cutting a 45 deg tapper down in a part. I have a ball drop to check the depth. When I run the program the ball drop was showing +.006 high on the ball drop. I checked everything and everything was right on the program side of it, I also checked the gaging of the tool to make sure that it was gaged right. Then I created just a ball endmill and ran that and it was right.

 

When using a user defined tool and you put in the dia. it should know what to offset, how does it know if it is a ball or not? On verify it looks like it offsets the path good to the part. I don't know what I am doing wrong. Some how it is not offsetting it right.

[Ron Branch @ Verisurf]

Ok then the question becomes what method did you use. There are 2 methods to define custom tools there is the 1.0 scale where you draw what ever tool to 1.0 from center line. So if you were making a custom 4" dia tool you would need to scale everything by .25 and vice versa if it were a .25 tool you would need to scale it 4 times bigger. Then you use a standard tool definition to the define the custom tool. Now the other way is to make a tool to scale and then define that tool by the diameter of cutting part. So you could have a .237 diameter tool with a .250 shank. You should define it as .237 in diameter and not .25. This method requires the Custom tool be used not a defined tool. The next question is how to do you test what is correct. Very easy. Make a round surface. Then do a surface toolpath like flowing one line. Then see by adjusting the diameter of the tool how your codes changes. Now you can figure out what it causing your error on your custom tool definition.

 

HTH