thread milling

[TonyK]

Does anyone know why the Major thread dia.

Dialog box grays out when selecting points or arcs? I used this tool path for the first time yesterday. I cut three 1/8-27 NPT test holes

first. When I was satisfied with the size,lead in

lead out I cut the cavity block only to have the

hole finish too large. When I checked the toolpath in my ops. manager I saw that the thread dia. box was grayed out. I tried picking on the hole dia. a point in the center with the same results. Why it work the first time I don't know. I got it to work by creating a line through the hole and selecting it's midpoint.

Has anyone had this problem with thread milling

or am I doing something wrong?

thanks

Tony

[Guest]

It greys out when selecting and arc because the arc provides the diameter definition.

 

If you HAVE to use it that way try creating only a point on separate level and use the points then you can enter a diameter.

 

I like to define my diameter and chain the arc.

[TonyK]

I tried useing a point and it grayed out.

I wanted too be able to alter the dia. to get the right fit for a pipe plug. Only arcs for the

inside dia. of the hole and the champfer were drawn in not the major dia. whitch is what the

TP cuts to.

[Guest]

I think the point you are picking is the center point of an arc.

 

You need to use only a point. I just tried it and it works as described

[Michael Sullivan]

John is right. The arc center cannot be the point you choose or the box will be grayed out.

[DavidSV]

I have found that if you define a threadmill operation with the centerpoint of an arc that it will always use that arc, even if you later delete the arc or change its size. You need to delete the whole thread mill operation and start over from scratch. Then you need to make sure that you use the selection button and select the point. Look at the icon when you select the points to make sure you are selecting the point and not the arc center. You will then be able to type in the major diameter box.

[gcode]

If you what to use point and enter your value,

just draw a point. If you have a circle, autocursor will pick the center of arc.

If you turn autocusor off, you'll get nothing

because there is no point there, just the center of a cicle.

I usually draw a circle and let that define the size.

If I want to change the diameter I use

F4 (analyize) to edit the size of the circle.

Here's a neat trick your operators will like.

Draw your circle the right size.

Define all your thread mills .01 or .015 oversize

(put .515 in the dia definition of a Ø.500 threadmill)

all your threadmilling will be .015 undersize

when the operator sets up with a D0 diameter offset.

He'll have .015 to play with to get a good thread.

[TonyK]

Got it now thanks. On the test cut I did pick

just a created point and the second time an arc.

 

thanks for the help

[TMozzone]

Also you could turn off the arc center setting in the cad settings config file, create a new layer and define all your arc centers with points on that new layer.

[ATG]

I use undersize geometry for my holes and then open the thread up with my over cut tab. Works Great....