I use "Process - Rough - Cavity" for facing all the time. You need to follow the same rules: The following procedure from the Help describes how to create tool path for a cavity or a core. The only difference is in the selection of the "Cut area Point" in step 2 1. Prepare for the Cavity step:
� Create a closed profile boundary to describe the stock material area. Specify the Level (of the profile) to the Z location of the material floor, and the Prof Top to the Z location of the material top. � Use Mesh-Planar Cuts, or Surface Machine-Contour (in the FreeForm Machining application only), to create planar profiles at each Z level that the mesh or surface is roughed. Set the Prof Top to the Z coordinate of the material top prior to generating the profiles. � Use Group to put the planar profiles into the active group. Tip � Use the Insert Property bar to set the insert position and clearance. Select With Step and assign a milling step to access the Rough toolbox. 2. Specify the Cavity geometry: � Select Process--Rough--Cavity. � In the Matl Boundary field, choose an element on the material profile to specify the perimeter of the material. � Specify a Cut Area Point to indicate the machining area. To machine a cavity, select a point near the center of the lowest planar profile. To machine a core, select a piont between the outermost planar profile and the material boundary. � Select the appropriate Path Type to rough the part: Spiral, Zigzag, or Linear. 3. Set the tool path parameters. � Before proceeding further, enter a value for all of the remaining parameters on the Pocket control panel. See the Field descriptions for parameter definitions. � Click the Params button to set advanced settings, if applicable, for the pocket cut. To select an active group of islands and notches, turn on the Avoid Grouped Islands switch. 4. Complete the Pocket step. � Click Accept to close any open dialog boxes, then select Go to start the operation. � Select the Undo to remove the last operation from the graphic view and database. Select Reset to return the input fields to their previous or default settings. � Use View--Show Path to verify the results. Fred Lauzus CAM Programming Coordinator CAD/CAM department 132 ** Ext-4117 -----Original Message----- From: Jon Baker [mailto:[EMAIL PROTECTED]] Sent: Tuesday, December 05, 2000 4:53 PM To: [EMAIL PROTECTED] Subject: [mfg-smartcam] Re: roughing surfaces Don't know if this ever really made it out. Its been 3 hours since I sent it, so I am sending again. If its a duplicate, Sorry guys Jon ----- Original Message ----- From: Jon Baker <mailto:[EMAIL PROTECTED]> To: [EMAIL PROTECTED] <mailto:[EMAIL PROTECTED]> Sent: Tuesday, December 05, 2000 10:43 AM Subject: roughing surfaces I have some parts that I just can't figure out the easiest/ fastest / best method for roughing. The part is an iges surfaces file, with what looks like a Jacobs taper at an angle sticking up on the top. I want to mill around the jacobs taper to get it somewhat to size and shape prior to putting it in a fixture to finish turn the angle. This will prevent a serious interupted cut condition in the lathe, as well as maintain the balance a bit better. I have fooled around with the various surfacing tools, with various cuts, but it doesn't seem to perform real well. What I would like, is almost like cavity roughing in a planar mode, that will avoid the island / peg / jacobs taper thing, but to do it as a facing, not cavity method. Like creating an EDM electrode. What I usually end up doing, is just laying down geometry around the part at various levels, and doing showcut to ensure that I haven't touched the actual part. This is time consuming and tedious, however my cut time is down under 10 minutes, as compared to over 20 for any surface roughing method that SC comes up with. Since I do the programming myself, it is "free" but the machine time needs to be minimalized. This is a repeat job so machine time is the big issue, and programming like this seems to be a standard issue that either smartcam or myself cannot seem to automate very well. Any suggestions? Jon Baker PS, I have hacked away and created a couple other surfaces so now you can see the basic idea I am trying to accomplish without my releasing customer drawings / engineering. I created two finish cuts with the one endmill, and that is what I want to finish on this step. Then the top part, I just want roughed in within .100 to .050 to keep it fairly even so that when I chuck up on the lower shaped surface in a form collet, it won't be so interupted on the lathe. The material shape at this stage is level 2, so enter that in showcut and you should be good to go. Thanks again for your input folks. Jon ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
