custom mill tools

[harmonson]

we are having a problem with custom tools, and are hoping maybe one of you can help us out. we have a lot of custom tools, but most of them are wider then 1 inch, and as a result we are not sure how to scale them. we have tried to scale them only in the x direction, so that our height remains the same, but then when we are in verify, when we put in our real numbers, it is very hard to tell weather or not the tool is doing what we want it to do. how do other people get around this problem? any advice would be appreciated. thanks a lot.

[Balbir]

Try to uncheck cutter compensation in control in verify and see if it works.....

[harmonson]

there was no difference when i did that. what does that do? i think maybe our main problem is that the tool looks so different in verify than it does in our drawings...

[Keith Graydon]

Go to the MasterCam help file topic:

"Creating a custom profile using an MC8 file"

HTH

-Keith

[harmonson]

i have looked at the help files extensivly. we have been able to draw tools, and i have scaled them down in the x direction, so that the radius in only 1", but often our real tools can be 2" wide at the widest point, and this is usually at the top of the tool. so we can shrink this to 1" for the drawing, but then when we use the tool, and put in our real numbers, we can not see if it is cutting our piece properly, nor can we see if we have 2 pieces next to each other if it will cut into the other piece. is this a stupid question, and should we just figure it out, and not rely on mastercam verification to help us out with this, or is there a work around? thanks.

[Keith Graydon]

Draw the tool fullsize. Then scale it in X AND Y so the RADIUS is 1.000. If I understandyour post you said that you were scaling it in x only.

-------------paste----------from help file.

Note: The X dimension of the tool RADIUS must be a value of 1.

-------------paste----------

-Keith

 

[harmonson]

we have been scaling it in the x only because if we scale it in both directions, then it becomes much shorter, and in verify it is then burried in our part. so we thought we could solve that by only scaling it down in the x direction, but maybe not... does this make sense? thanks.

[Keith Graydon]

Try scaling both as you loose the correct aspect ratio of the tool when MasterCam applies it to the geometry.

Define the tip/centerline of the tool at

0,0,0.

also: check Z height of the stock in Verify. Make suure it is set to Z 0.0.

-Keith

[harmonson]

i am slightly confused by your last statement:

"also: check Z height of the stock in Verify. Make suure it is set to Z 0.0."

i made all my z values = 0, and i got a failure in stock definition. we like to predefine our stock so we can see how it will actually run at the machine, often when mastercam defines it for us, our lead in lead outs are hard to see weather they will ram the wood or not. thanks.

 

[Keith Graydon]

Harmonson;

We -usually- program from the top plane of the work. It follows then that every move into the work is in the -Z direction. With that in mind, try This::::

1. From operations Manager, Select all your toolpaths that you wish to verify.
2. press the verify button
3. Press the far left button (marked (?)) on the verify controls and you will be pesented with these options.-- see attached .jpg.
4. In the boudaries section press the SCAN TOOLPATHS button.
5. Now, look at the dimensions that have been inserted in the X,Y,Z and margin fields.

   Z Minimum is the Depth of the deepest tool with reference to Z0.

   Z Maximum is the Height of the highest retract with reference to Z0. X and Y boundaries a drawn from the centerline of the tool (left and right extents)

6. Type in any values that will work for you to define your stock. this is where I meant to set your Max Z value at 0.0. Set your minimum Z value at least to the depth of your deepest cut.

BTW. Are you programming an actual Z depth in the toolpath or are you leaving it at Z0. in MasterCam and managing it at the machine? If you are leaving it at Z0.0 Please give it the same depth (or thereabouts) that you'll me using at the Machine. Whew

HTH

-Keith

I hope i typed all this right..........

[This message has been edited by Webmaster (edited 06-20-2001).]

[Allan Brown]

In a nut shell, you need a custom tool profile "normalzed by the radius" for each tool you use. The custom tool definition was created to allow scaling based on the tool diameter. In practice if you need the custom profile to be exact including features in the Y direction (e.g. flute length), you need to draw the tool profile sized correctly, then scale everything by 1/R, where R is the tool radius. When Mastercam applies the tool diameter to this "normalized" profile you get your original tool back.

[harmonson]

ok, i will try and answer your question and/or explain myself better. sorry, i am a little slow at this stuff...

the way that we program is that we say that the bottom of our stock is at 0. then if we want to cut below our stock we would set our depth to say -1/8 or -1/16. if we want to leave some on, then we would set our depth to 1/4 or something like that. our top of stock is a positive number, however thick the stock is.

i tried to do it the other way, and let the top of stock be at 0, and have our depth be negative and tried to verify that to see if it would work, as well as scaling my tool in both x and y. when i did this, my tool was sunk in the piece because it was too short. it still did not look like what i had drawn.

also-we like to draw a rectangle the size of our stock so that we can use the select corners option in job set up. the reason we do this is to make sure our lead in/lead outs are ok.

we are not programinng at actual z depth, we have our post set up so that we can say the bottom of the stock is at 0, and the post will then take care of calculating the actual numbers. i hope this makes sense. i appreciate your help and time. also one last question-- what is this: "

[Keith Graydon]

Hi,

the list=1 was a typo on my part. I was trying to force a numbered, bulleted list using "UBB code".

1. Like
2. this

I didnt close it correctly. It should have been hidden.

Oh, I just thought of one more thing..

Is your depth of cut with your special tool deeper than the length of the tool as defined? If it is you can rough your way down by using a dummy pocket or faceing routine then use your tool to finish.

-Keith

[This message has been edited by Webmaster (edited 06-20-2001).]

[harmonson]

the depth of the cut is not deeper then the length of the tool as defined. if the length of our tool is 1.8125, i can not seem to make the stock bigger then 1.567 with the depth of my cut being 1.567 as well or the tool will be burried. after the tool was scaled down, so that the radius was one its height was 1.568. so i guess my question is does mastercam scale custom tools up to size, it seems like it only offsets them in the x direction... thanks.

 

[Fred from Université de Sherbrooke]

Harmoson,

Just a little thing to help you with custom tools: When I'm not sure if the tool is well draw, I go in backplot, (make sure your tool appearance is plain)and do a SNAPSHOT. This way you can analyse your tool and be sure of your settings. Hope this help!

------------------

***FRED***

[harmonson]

thanks fred. i did this, and our tool seems to be ok. i think the problem we are having is that mastercam does not seem to scale our tools. so that once we have drawn it and scaled it down so that the radius in 1, when we go to actually use it and our real radius is say 2, it will not scale the tool up, rather it seems to offset it from the part 1". the reason this is slightly problamatic to us is that we can not see if the tool is cutting the wood properly or not. does this make sense? are we the only ones with this problem because we are over looking some extremely simple detail? thanks a lot.

[Guest CNC Apps Guy 1]

I've been building tool libraries for about the last week and a half. Our tools are simple enough but we also verify/backplot with the tool, holder and spindle nose.

What has worked for me to accurately see what is going on is to model the tool/holder/spindle assembly profile to exact size. Save it in your /mcam8/mill/tools/ folder. Then go to NC Utils and create a tool, the type NEEDS to be "Undefined". On the parameter page you need to get the geometry file that you saved in the /mcam8/mill/tools/ folder. Go back to the First page specify the compensation diameter, and then select the "Custom" button on the right side. You shoudl then see your tool.

Hope that helps.

------------------

James M.

Mastercam Enthusiast

[This message has been edited by James Meyette (edited 06-27-2001).]

[harmonson]

james-thank you thank you thank you! i think that has been most of our problem. that makes so much sense, and it works...i guess this is why we need to get to class. thanks again.

[Guest CNC Apps Guy 1]

Glad I could help. Take those classes.

------------------

James M.

Mastercam Enthusiast

[Tony]

James

With all your help here and the way I have perceived you through your writing's....

I picture you as the "Orson Wells" of Mastercam...except you race BMX I cant quite fit that into the Orson Wells picture!

Many thanks again

tony

[harmonson]

heh- i either spoke to soon, or more probably, i have another stupid question. the tool i am working on now does not seem to woek. the widest part of it is 2.194", the other one i tried out first was not even 1.5" wide, so i am wondering if it is because it is so much wider. i have checked it multiple times, and it is connected everywhere, and there are no splines, it is made of 4 arcs and 9 lines, so i am not sure what i am doing wrong, although im sure its something easy... thanks again.

[Guest CNC Apps Guy 1]

I will attempt to link to a picture. Thisy type will not work because if you think of it in terms of how a tool actually cuts, you'll understand.

(You'll have to go into CADCAM's ftp site to get the pictures. They are the only JPG's in there and are named so you'll know what they are.

ftp://ppcadcam.com/Mastercam Forum/Tool

Will Not Work Correctly.jpg

This type will work correctly because there is no "Self Intersections" for lack of a better term.

Hope this helps.

ftp://ppcadcam.com/Mastercam Forum/Tool Will Work Correctly.jpg

I'm only 31 so Orson's out of the question, but I do like my cave, errrrr, office dark and with Heavy Metal Playing in the back ground. No facial hair either, but I do have a "Flat Top". If I can find an electronic picture, I'll post it if somebody wants me to.

 

------------------

James M.

Mastercam Enthusiast

That Didn't Work.

[This message has been edited by James Meyette (edited 06-29-2001).]

That Didn't Work Either

[This message has been edited by James Meyette (edited 06-29-2001).]

Guess I gotta do things the old fashioned way.

[This message has been edited by James Meyette (edited 06-29-2001).]

[harmonson]

i think i understand why the first tool wouldnt' work. i put a picture of a tool we are trying to put in our library, that just will not work. it is probably the way i have it drawn or something simple like that. it is called: should it work.jpg

thanks for your responses.

[Guest CNC Apps Guy 1]

That tool won't work. It's hard to explain. E-mil me and I'll explain why. I can attach pictures there.

------------------

James M.

Mastercam Enthusiast

[harmonson]

james-

there was 1 tiny little overlapping entity at the bottom of the tool.

arrrrgh!!!

thanks for all your help.

-emily