Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Custom Lathe Grooving Tool

Kampfzentrum

By Kampfzentrum,
in Industrial Forum

 Share

Recommended Posts

Kampfzentrum Explorer

Kampfzentrum

Posted
Posted

Morning gents, got a perplexing issue here. I'm new to a company that has handed me the responsibility of creating a full graphical tool list for their VTL. I've drawn the tool up and saved it to my own tool database, but when I insert it into an operation, I get it coming in inverted like this. I've attached how it comes in along with the dialog box where the tool geometry is defined.

Now, I'm sure someone is going to come out and tell me something simple that I missed, so I must state: I am new to the lathe/VTL world. Any tips moving forward would be great. But for now just solving this mystery would be great.

Thanks guys.

Groovemania1.png

Groovemania.png

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Whenever I am setting up a "new tool" in Mastercam Lathe, I always use the "Draw Tool" button. That will show you the orientation of the tool, and how it "sits" on the machine. The issue you are having, is "VTL" is a weird animal in Mastercam. It depends on if you are using "World Z = Lathe Z", and how the Machine Definition was built.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted (edited)
3 hours ago, Kampfzentrum said:

What setup screen would you like to see? I am not sure what screen you are requesting. I personally drawn the tool just as you described. I am not sure why it is inverting it like it is.

 Zip2Go posted.

 

2039916A.ZIP

The  tool has been defined incorrectly. The center of the Radius should not at the Origin. The tool should be defined at the cutting edges for the X and Z Zero. The grooving operation set to OD grooving not Face grooving. The tool is drawn to cut in an OD fashion not a face grooving fashion. The tool needs to be rotated and moved to the correct place and then it should be good to go. I just turned it 90 degrees. You may want to turned 90 and the mirrored I don't know I just did a quick and easy way to help you along.

Here is the file back with the tool defined correctly and the correct tool orientation picked also.

HTH

 

Edited by C^Millman
Changed the file added it in a new posting below
Link to comment
Share on other sites
Kampfzentrum Explorer

Kampfzentrum

Posted
  • Author
Posted
19 minutes ago, C^Millman said:

The  tool has been defined incorrectly. The center of the Radius should not at the Origin. The tool should be defined at the cutting edges for the X and Z Zero. The grooving operation set to OD grooving not Face grooving. The tool is drawn to cut in an OD fashion not a face grooving fashion. The tool needs to be rotates to the correct place and then it should be good to go.

Here is the file back with the tool defined correctly and the correct tool orientation picked also.

HTH

5th Axis 2039916A.mcam

I still really am lost as to how you got the tool orientated correctly. I deleted the operation, deleted the tool completely, edited the tool and set the cutting edges for X0 and Z0, re-created the operation, imported the new tool, chose a "face" groove, and yet the tool is still cocked. I cannot see what you changed to get that dang thing orientated the right way.

Link to comment
Share on other sites
Kampfzentrum Explorer

Kampfzentrum

Posted
  • Author
Posted
10 minutes ago, K2csq7 said:

If possible I'd wait for 2019 to create a full tooldb, 3d tooling is a gamechanger. 

I'm not even doing 3D, I'm just doing a wireframe and it seems like madness. I honestly can only blame myself as I haven't had a formal education in any of this. I'm really just trying to wing it.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
On 2/20/2018 at 10:18 AM, Kampfzentrum said:

I still really am lost as to how you got the tool orientated correctly. I deleted the operation, deleted the tool completely, edited the tool and set the cutting edges for X0 and Z0, re-created the operation, imported the new tool, chose a "face" groove, and yet the tool is still cocked. I cannot see what you changed to get that dang thing orientated the right way.

I took your original tool and I used the lathe tool manager to export to a level. That is Level 100 on the file I posted back up. I did my Transfrom Rotate and rotated it the 90 degree. I then used dynamic to move it in X and Z the .0225 needed to get the edge where it needed. I then changed from the 5 position you picked originally and used the 1 position. I again threw this together quickly. I don't know how you plan to touch off the tool or anything like that. You also need to go into the setup of the tool and tell the setup the tool will be vertical or horizontal you had chosen Vertical which again was to support OD grooving not Face grooving.

When I am talking about Setup for a Lathe tool there is the last page I am referring to on this picture.

Image Link #1

If you click on the Question mark there is help that defines what each thing means.

Image link #2

How are you going to mount this tool in the lathe? Decide that then match that in Mastercam. Your MMD doesn't tell me you have a Turn/Mill with B axis where you will moving the B axis to turn the tool 90 degrees so I have to assume you will mount it horizontally on the machine. If that is the case then you have to match that on your tool in Mastercam. It can only go by what you define and if you define it one way it cannot move it the right way.

I have never taken the 1st Mastercam class all self taught, but I have taken the time to read a lot of the help.

  • Like 1
Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
1 hour ago, K2csq7 said:

The tool definition for 3d tooling is completely different from legacy custom tools. MUCH simpler. 

For example, instead of trying to make sense of those 16 radio buttons AND the setup tool window's settings in legacy custom tools, in 3d tooling....... this;

 

3d.png

That is a great improvement, but it doesn't help him solve his immediate problem.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted
On 2/21/2018 at 5:25 AM, Kampfzentrum said:

Call me crazy... But why does it seem that during any backplot simulation the tool that I created (that you edited) takes off more stock than the feature itself? Tool looks to be plunging into areas it shouldn't be.

Yes sir you are correct I forgot to do one step. On the last page of the Define tool is a tool Clearance page. I didn't do it so the tool is not full defined yet.

On the last page need to click on the tool clearance to set the groove tool.

https://www.dropbox.com/s/1yhm5r7u56hyc5w/LatheToolSetup_2.png?dl=0

Don't do the logical thing and run the tool scan you will get weird results.

https://www.dropbox.com/s/z7ik1lb6n6xmtqr/LatheToolSetup_3.png?dl=0

Manually type in the Width and Height as the same thing and you then should be good to go.

https://www.dropbox.com/s/4yu1gyki2mk8qvd/LatheToolSetup_4.png?dl=0

I would change the percentage of step over to something like 40% or 50% and I would peck groove to get away from stringy chips. Here is a screen shot after the adjustment and you are where you expected to be.

https://www.dropbox.com/s/m6nh6fgg26xowme/LatheToolSetup_5.png?dl=0

I removed the file from above and have a new file here with the changes. Running out of room on the forum so these pictures and file will disappear in the next couple of week.

5th Axis 2039916A

  • Like 2
Link to comment
Share on other sites
Kampfzentrum Explorer

Kampfzentrum

Posted
  • Author
Posted

OK, let me ask another question.

In the case of a standard turn/face tool on a VTL. Most people would run a turning tool on the left side of the part using M04. However, because of the type of parts and the rigid system put in place, these guy manually program parts where the tool crosses over the centerline of the part onto the other side to face and bore using M03. I am not seeing this ability to change this on the fly, where is this parameter?

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...