Do you see anything wrong?

[Thoob]

I drew this custom tool for a threadmill. I saved it in the tools folder and when I call it up for a part, it is smaller than what I drew it at. The profile looks right and it accepted it as a custom tool, its just smaller.

[Josh Kinney -Elite Engineering]

Has to be drawn at 1" Radial and then it gets scaled in mastercam.

[Thoob]

I'm sorry i don't follow. 1" radial?

What has to 1"? What about other dimensions?

 

What I did, not sure if its right, I went into properties and changed it to undefined tool and put the actual diameter in. Not sure why I would have to do this but it seems to work as it brought the threadmill to the proper size.

[Colin Gilchrist]

First, make sure that you delete the centerline. It isn't needed on a custom tool shape. Just the outside profile starting at the origin, and drawing the outer shape of the tool.

 

The help file has notes about drawing the tool at 1" on the diameter, so that the shape can be scaled. I recommend you do not do this. Just draw the tool profile at actual size, and make sure you enter the correct diameter when defining the tool.

[Thoob]

I understand the centerline isn't needed, however it does not affect the custom tool does it?

I did do what you said about drawing the actual profile and defining the actual diameter. I mentioned that in my last post so I will assume its ok, lol. Thanks guys.

[Josh Kinney -Elite Engineering]

Sorry, Diameter. Couldn't remember off the top of my head. I always found custom tools to be a pita.

 

The centerline should make it fail.

 

-Josh

[Thoob]

No it still works with the centerline. I believe if it was a solid line, it would fail. I never removed it and it still accepted it.

[Josh Kinney -Elite Engineering]

Your right, that's strange....

[Buddy J]

............Just draw the tool profile at actual size, and make sure you enter the correct diameter when defining the tool.

 

 

In the case of a form or multistep tool, I'm guess that this would be the largest diameter or the diameter at the tool tip?

[Colin Gilchrist]

In the case of a form or multistep tool, I'm guess that this would be the largest diameter or the diameter at the tool tip?

 

Yes, but it depends on what you are trying to do, and if you need to use cutter compensation with the tool or not. Most of the form tools I've used were for ports, so I would usually just enter the diameter as the "reamer" portion of the tip and call it good...

[Jayson Kramer]

Your right, that's strange....

not really as you used to have to make it when doing custom tools and it had to be yellow color 14. but not needed thses days I still do it as this the way I was shown YEARS ago.

[Rotary Ninja]

I always draw my tools with the centerline and have no problems. I draw all my tools to scale then scale the compensation point to 1". I will post the way I do it for anyone that finds this thread and needs to know how to create a custom tool.

 

So if I were drawing a .750" threadmill...

 

Draw the radius of the tool to scale and dimension the point where you will be compensating from...

 

After you have the tool drawn select all the geometry and Xform>>>Scale. In the scale value field enter 1.0/"the point of your tool you will be using compensation from". In this case the tool is a .750" threadmill. The rad of the compensation point is .375". So the value to be entered is 1.0/.375.

 

This will yield this:

 

Save the file into your Mill/Tools folder. You can leave the centerline and the dimensioning. It won't make any difference.

 

Now in the tool settings I would use a key cutter for this tool. This allows me to enter the flute width (thickness of the cutting head). This is just for reference for the next guy who has to find the tool I used in our mess of a tool cabinet. Click the "Custom File" radio button and select to the tool file you just saved.

[MrFish]

Spot on Rotary Ninja, this is how we always do it. But I add one extra step of saving the profile at full size as a dxf first to be used for custom tool generation in vericut, then scale it back to 1.000 and save as a mastercam file.

[crazy^millman]

Way I have done it for almost 10 years is with a Centerline. It has always worked for me that way.

 

Ninja good to see the effort you put into this thread thanks for sharing your knowledge with others.

 

HTH

[Rotary Ninja]

Ninja good to see the effort you put into this thread thanks for sharing your knowledge with others.

 

Thank you. I have seen this topic come up a few times in the past so I thought I would post this up.

[Thoob]

I agree, thank you for that tip. Appreciate it.

[MoMo1108]

From what im told you will no longer have to scale it in x7 fyi

[Thoob]

That would be nice. Doesn't make any sense to me why it has to be scaled. I still don't understand the whole concept of drawing it at 1".

[MotorCityMinion]

The tool does NOT have to be SCALED. I draw half the tool profile accurately, on center and that's it.

[Jayson Kramer]

The tool does NOT have to be SCALED. I draw half the tool profile accurately, on center and that's it.

You are correct but he was showing another way to do it is all.Just another tool in allot of peoples tool box of MC

[Mick]

I stopped scaling custom tools a while ago. One less step to worry about

[Scott Lundin Shopware Inc.]

I always use the "undefined" tool category then you don't have to "scale" your on-size tool drawing. I think it is when you use any of the other categories that you will have to scale it as shown a few posts above.

[MotorCityMinion]

Like I tell my boss... "There's only so much room between my ears. Keep filling it with useless or redundant information and something good is going to get lost."

 

Not saying that was useless data, it actually was a great presentation.

[Rotary Ninja]

I don't use undefined tools. If I am using a port tool I want to use a dwell. So I will define my custom tool as a counterbore. This gives me options similar to the counterbore to use with my port tool. I already mentioned that I use a keyway for my threadmills to be able to define the head thickness along with the diameter. I like having tools defined more closely to what I am using. You cannot do this with an undefined tool.

 

It's not like you have to break out the trig calculator to scale a tool anyway MCM

[MotorCityMinion]

Good thing too, trig was one the good items forced out of my head by my boss a long time ago.