Continue to Site

Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Milling Pockets from Start Holes

anandel

New member
Hi all,

Here's what I am trying to do. I have a plate with some pockets to be milled out (pls. see the attached pic). Since I don't want an 1/2" end-mill to plunge right into the part, I want to drill some start holes inside the pocket first and then would like to start milling from there. The holes may be created in some arbitrary location (shown points)inside the pocket and the depth same or shallower than the pocket.

View attachment 1239

I created the milling sequence (after creating the drill sequence) using Volume -> Window. Now, how can I say Pro/E to move the tool to that location and start milling from the hole. Even if I pick the point as 'Start' point, the tool comes down on it, but retracts and starts milling from the default location.

I am relatively new to Pro/Mfg. Is there something really basic that I am missing? Gurus, pls help.
I'm using WF 2.0 M110.

Thanks
 
Instead of using start holes I sometime use the ramp parameter. You can set the angle you want to ramp down and you can also specify a feed rate for ramping. If you want to use a start hole then try this. Define an axis perpendicular to sketch plane anywhere with in your manufacturing window. You may need to move the axis up the model tree so that it is before your mfg. window. With axis defined and your NC sequence active go to SEQ_SETUP and put a check-mark on build cut/DONE. Now select approach, use whole volume YES, select AXIS from the menu then select the axis you defined earlier. Do this for the exit as well. This also works well with profiling. Let me know if you need additional help.
 
If your start point, ( the holes), have an axis, you can you this in the "mill-volume" sequence. After you tool path has been created, pick "sequence setup", "build cut", and "done". When the "build cut" menu appears, pick "approach", "whole volume", "axis", and done. Now select the axis that you want to start from, and pick"done_return".


You can also create an "end point" by doing the same thing as above except pick "exit" instead of "approach". By doing this each slice will end up at the start point of the next slice, so the tool will plunge inside the hole that you created previously.


You may also want to change the sequence parameter "APPR_EXIT_HEIGHT"to "DEPTH_OF_CUT" instead of "RETRACT".


Good luck Anandel
 
Thanks very much both of you. It did work. But then, it looks like that there is a limitation of having to make one 'Window' for every pocket. For example, if I have 5 similar pockets, seems like I'd have to create 5 different windows and as many sequences so that I can have 5 approach axes and exit axes, right? I don't mean its hard to do or anything, but just a thought.

Also, as a related topic, what is a good way to do an 'open pocket' milling (both with a depth & straight thro')? I tried with Volume->Window milling, and also defined my approach walls so that the cutter can clean out the edge of the pocket. But, the cutter doesn't want to come out of the 'window' except for the entry and exit passes. Is this the right way or is there any other better way to do an open pocket? I hope I explained the problem right.


Thanks again.
 
The answer to your first question is yes, you have to define each window and itsapproach & exit axis. Sounds likea job for a UDF.


I'm not sure I understand your related question. Blind and thru pockets should be set-up the same as what you just learned. Why are you defining approach walls to clean edges? Why do you want cutter outside of window? The window is used to contain the cutter. Are you using feature edges from your mfg. reference model to define window perimeter? If you are using feature edges to define window and your ROUGH_OPTION is set to rough&profile you should get a nice clean pocket. Please explain more.
 
I was meaning to ask about a pocket as shown in the picture below:

View attachment 1249

I am not sure if an open pocket like this can be milled in a similar way as a 'regular closed pocket' ('Open' in terms of its edges). I created a window using the edges and used that for milling, which as you explained, contained the cutter inside. Then I defined the outer curve as the approach wall. Except for the entry and exit passes, the cutter was milling only inside the window. If it doesn't mill past the outer edge, it might leave some kind of a ledge in there right? Is there any other way of doing this?

Is there any other important Parameters that I need to set to do this type of milling?

Thank you very much. I appreciate your time.
 
The image you have attached helps. Okay you might want to try3 things here.


1. Ifyouwant to use a mill window you will need extend your window edge, extend the edge with no wall by at least the cutter diameter, however this method will cut air.


2. If you choose not to extend window youwill needa profile sequenceto finish the pocket walls.


3. Difine your own tool path using a trajectory sequence. This option is pretty cool once you get the hang of it.


Let me know if you needhelp.
 
anandel said:
I was meaning to ask about a pocket as shown in the picture below:



View attachment 1251



Try to create the actual VOLUME instead of WINDOW. It's a bit more work
upfront, but it's much more flexible - especially with open pockets you
can specify the APPROACH WALL (one or more) and you cutter will enter
and exit through there. Works very well. For pocket like shown, it'll
be a snap, all you need to do is to CREATE VOLUME using SURFACES with
FILL option checked - pick only the bottom one and pick it again to
"fill" the holes. YBefore you exit the VOLUME CREATION menu, you may
need to TRIM riht avay the top surface of the created volume by the
value of your CLEAR level (I use .100") because it tends to stick out
above your part. All done.

Same with closed pockets - you can use entry axis at will. VOLUMES are
more elegant (IMHO) than WINDOWS, however it depends on the application.



Please let us know if it worked for you.

-mark
 
Thanks for all your suggestions Mark & Rick.

Mark, I tried it and it works, but ofcourse I have my own share of questions and troubles. First, the Trim while creating the Volume, does not work for me, Pro/e gives some kind of an accuracy error. I didn't change the part accuracy from the Pro/e default either.

View attachment 1256

Second, as in the previous post, wouldn't it be nice to get the cutter come past the open outside edge? Which I guess is not possible with volume milling.

Rick, I tried the trajectory milling. What I found is, the cutter just follows the trajectory and it's gonna leave an 'island' of stock outside of it right? Is there anything that I am missing as a parameter setting?

Last, for Approach and Exit should I only use axes or I can use datum points? I thought it'd be little quicker to create points than axes.

As a general question, in a typical situation like this, what is the factor that basically categorizes the type of milling to be used? I am doing this exercise for our mfg dept people. I'd like to create some UDF-s and tell them 'this is when you should use this UDF'.
I understand that there is a lot of different ways of doing a particular operation, but just trying to draw a line that certain ways are generally acceptable.

Thanks very much every one of you guys. I really appreciate all your valuable inputs.
 
The beauty of a trajectory sequence is that the tool follows your sketched curves. Redo your trajectory so that it leaves no island.<?:namespace prefix = o ns = "urn:schemas-microsoft-com:eek:ffice:eek:ffice" />


As far as Approach & Exit goes I found that points are easy to make but had better success using datum axis. The Pro/E menu selection can be misleading sometimes. I don't know if you notice but when defining an approach pro/e says "select an axisto specify start point".


Your last question is a tuff one to answer because it really depends on how you guys do things in your office/shop. I personally like to use a mfg. windows where my cutter ramps into the workpiece. I tried using mill volumes beforeand found that mfg. windows work better for what Ido here.My suggestion toyou is keep testing the many different ways to machine pockets till you find something that works for your company. Let me know if you have more questions.
 
anandel said:
Mark, I tried it and it works, but ofcourse I have my
own share of questions and troubles. First, the Trim while creating the
Volume, does not work for me, Pro/e gives some kind of an accuracy
error. I didn't change the part accuracy from the Pro/e default either.
.....
Second, as in the previous post, wouldn't it be nice to get the cutter
come past the open outside edge? Which I guess is not possible with
volume milling.



Use OFFSET, not TRIM, sorry about the confusion - my memory isn't that all great.

OFFSET will let you "move" any face of the volume in either (in or out)
direction by any amount you wish. Very convenient feature, you'll love
it.



As far as getting the tool outside the open edge, it's easy - again,
OFFSET the open wall to the outside by desired amount and watch your
cutter obey :)



There's even an option to OFFSET by TOOL_RADIUS, but you can't modify it later, should you need to switch to another value.



I hope it helps,

-mark
 
anandel said:
Thanks very much both of you. It did work. But then, it looks like that there is a limitation of having to make one 'Window' for every pocket. For example, if I have 5 similar pockets, seems like I'd have to create 5 different windows and as many sequences so that I can have 5 approach axes and exit axes, right? I don't mean its hard to do or anything, but just a thought.


You can create a single mill window consisting of multiple closed sketches. Then, when creating the sequence use the "Order Regions" function (in Build Cut? I'm not at my workstation). You can then define an approach and exit for each region as well as specify the most efficient order in which the pockets should be processed. This way you have a single sequence for multiple pockets. By my last count it took 14 mouse clicks per region to set approach and exit. Tedious but useful when, for example, counterboring a bunch of holes by interpolation where you want to plunge down an axis..





Regards
 

Sponsor

Articles From 3DCAD World

Back
Top