Bodcad programing

[TDCMS]

I have bobcad/cam v24.
I have used it to program my mazak already.
Now I am progrming a helix with it and the tool path
as it run the tool lifts up them back down runs some more
then back down.
In the sim as well as on machine.
Can someone help me to get this fixed ?
Been on tech support with little help in fixing it.
Been down for days running out of hair.

[Machineit]

Post your file here for people to look at. Go to the file. right click and click send to and zip. Then attach it to a post.

mike

[TDCMS]

Here is file

[aldepoalo]

TDCMS,

It looks like you want helix down on the first op to clear out the stock. You can do this with BobCAD CAM.

When you are profiling with BobCAD you have 3 patterns

Standard

Contour Ramping

Side Roughing

In this example you want to use contour ramping. This will allow you to helix down and a depth or angle you define.

I made the changed to your face feature and have attached the file. Please let me know if this helps.


If you can not open my file then you are not running the current version of BobCAD-CAM 24 download and install the update from here: Software Updates | BobCAD-CAM

[aldepoalo]

I forgot to attach the file, sorry.

[aldepoalo]

Cutting Profiles with BobCAD-CAM

Profile cutting is so common almost any 2D part you machine requires this type of tool path. From finishing the wall of a pocket to cutting around the outside shape of a part, profiling is essential.

We offer 3 types of profile options that accommodate for different profiling needs. These options can be found under patterns of the Mill 2 Axis Wizard

Standard:

Our standard profile cuttings allow for a rough and finish tool, stock for finish, lead in / out options and step down in z. This is the most common profile cutting tool path.

Watch a video to learn more: Standard Profile - adepoalo's library

Contour Ramping:

This option allows you to ramp the tool around any profile. Common uses are for helical milling & slot milling. You control the angle of cut or a step down distance.

Watch a video to learn more: Profile Contour Ramping - adepoalo's library

Side Roughing:

Allow you to walk the tool in to a profile. Works best where you have more stock to cut then the cutter can take on a single pass.

Watch a video to learn more: Profile Side Roughing - adepoalo's library

With all profile cutting features you have compensation options, Allowing BobCAD to offset for the cutter, or to call cutter comp (G41 G42). These compensation options allow for wear comp, cutter comp, and center line cutting.

Using our profile tool path you can cut slots, shoulders, letters, holes, filets, t slots, dove tails, form shapes and other common every day 2D milling features.

If you have any questions please let me know.

[aldepoalo]

TDCMS,

After looking at your post processor Mazak_VTC_Rev1 Which can be downloaded from: CNC Machine Post Processors | BobCAD-CAM

It doesn't look like the post file is setup for 3D arcs for 2D cutting. This is the code that I get:

O010
G1 Z1.621 F10.
X2.4425
G17 G3 I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
I-2.4425 J0.
X2.4421 Y-.0416 I-2.4425 J0.
X2.4425 Y0. I-2.4421 J.0416
X2.4421 Y-.0416 I-2.4425 J0.
G1 X.1924 Y-.0033 Z0.
G0 Z2.121
M99
I


I don't see any Z values so that's not going to work...

You'll need to edit your post and the following blocks are where 3D arcs setting are in your post.

64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,arc_center,feed_rate

65. Arc move YZ.
n,g_arc_plane,g_arc_move,y_f,z_f,arc_center,feed_rate

66. Arc move XZ.
n,g_arc_plane,g_arc_move,x_f,z_f,arc_center,feed_rate

On Block 64 it's not calling any Z movement.

You can

1) Post with line segments - Setting in the posting option of the profile features

2) Edit the post to output the Z values.

64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

Having your 64 block look like this will post Z movements in contour ramping.

Sample Code:

O010
G1 Z1.621 F10.
X2.4425
G17 G3 Z1.4736 I-2.4425 J0.
Z1.3262 I-2.4425 J0.
Z1.1788 I-2.4425 J0.
Z1.0314 I-2.4425 J0.
Z.884 I-2.4425 J0.
Z.7366 I-2.4425 J0.
Z.5892 I-2.4425 J0.
Z.4418 I-2.4425 J0.
Z.2944 I-2.4425 J0.
Z.147 I-2.4425 J0.
X2.4421 Y-.0416 Z0. I-2.4425 J0.
X2.4425 Y0. I-2.4421 J.0416
X2.4421 Y-.0416 I-2.4425 J0.
G1 X.1924 Y-.0033
G0 Z2.121
M99

* This format may need a K not a Z which can be adjusted in your post processor.



You can change the post yourself, watch this video to learn more:

BobCAD-CAM’s post processor can be easily edited. The post controls the g-code output. Common edits that users make to their posts include start up codes, tool change codes, and where the machine returns to after cutting. Below is a video that covers how to make changes to the post processor.

http://www.youtube.com/watch?v=0LZr7I5lTH8]How to make a simple modification to a post processor BobCAD V23 - YouTube

How to edit the post processor:

http://www.youtube.com/watch?v=fyyViHren4I]BobCAD-CAM V24 Getting Started 15 of 15 - YouTube


More information on BobCAD-CAM can be found at: BobCAD-CAM SUPPORT TICKET SYSTEM - Knowledge Base


Or you can have BobCAD make the changes to the post for you

About Post Processors

BobCAD-CAM provides standard Post Processors free of charge. Modified or Customized Post Processors are covered under our Technical Support Memberships. To view the available options please click here.

A Post Processor is a unique “driver” specific to the CNC controller it’s intended to work with. The Post Processor controls the format of the G-code produced by BobCAD-CAM.

For BobCAD-CAM to effectively run your CNC machine you must choose the proper post. Use the menu below to choose the correct post for the version of BobCAD-CAM software you have, and the machine controller you want to post to.

BobCAD-CAM provides free Post Processors to all of it’s customers. There is no limit to the number of post you may download and use with your BobCAD-CAM software. We have many post configurations ready for download.

Post Request | BobCAD-CAM

[aldepoalo]

The problem here was the spiral tool path not following the curves of the solid.

When working with vertical or near vertical walls the equidistant tool path is the better option, allowing the tool path to follow the models curvature.

If TDCMS has time it would be great to show the difference in the part finish from the spiral tool path to the equidistant with some pictures.

[aldepoalo]

In this case if the tool walks the wall of the cavity it will cause tool marks which in not desirable. These tool marks are made due to the change in direction of the cutter.

Check out the sample cut part and the customers sample.

[aldepoalo]

The solution is to keep the tool on the bottom of the surface and not have it climb the wall. Also to make sure the pass the tool makes on the wall is climb cutting and done in 1 clean pass.

I had to make some changes to the boundary as to avoid the tool walking up the wall and changing direction. Once this was done the part wall finish was 10 X better.

See for yourself!

[TDCMS]

A big thanks go's out to Al from bobcad support.
If you look at posts I was spinning my wheels
on this part my short time using Bobcad didn't help.
But having CNC Zone and Al I was able to run the parts
and get the finishes I needed to move on.
Thanks again GUYS!
Doug
TDC Machine